Autodesk Mechanical Desktop ® ® User’s Guide 6 20507-010000-5020A May 3, 2001
Copyright © 2001 Autodesk, Inc. All Rights Reserved This publication, or parts thereof, may not be reproduced in any form, by any method, for any purpose. AUTODESK, INC. MAKES NO WARRANTY, EITHER EXPRESSED OR IMPLIED, INCLUDING BUT NOT LIMITED TO ANY IMPLIED WARRANTIES OF MERCHANTABILITY OR FITNESS FOR A PARTICULAR PURPOSE, REGARDING THESE MATERIALS AND MAKES SUCH MATERIALS AVAILABLE SOLELY ON AN “AS-IS” BASIS. IN NO EVENT SHALL AUTODESK, INC.
Contents ® ® Part I Getting Started with Autodesk Mechanical Desktop . 1 Chapter 1 Welcome . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 3 What is Autodesk Mechanical Desktop?. . . . . . . . . . . . . . . . . . . . . . . . . . . . 4 Making the Transition from AutoCAD . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Migrating Files from Previous Releases . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 5 Data Exchange. . . . . . . . . .
Mechanical Desktop Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .30 Updating Help Files. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .30 Product Support Assistance in Help . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31 Updating the Support Assistance Knowledge Base. . . . . . . . . . . . . . .31 Learning and Training Resources . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .31 Internet Resources . . . . . . . .
Applying Geometric Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 88 Showing Constraint Symbols. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 90 Replacing Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 91 Applying Dimension Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 94 Creating Profile Sketches . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 96 Adding Dimensions . . . . . . .
Chapter 9 Creating Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 167 Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .168 Basic Concepts of Work Features . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .169 Creating Work Planes. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .170 Editing Work Planes . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Using Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239 Active Part Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239 Global Design Variables . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 239 Creating Active Part Design Variables. . . . . . . . . . . . . . . . . . . . . . . . . . . . 239 Assigning Design Variables to Active Parts . . . . . . . . . . . . . . . . . . . . . . . .
Chapter 14 Creating Shells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 345 Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .346 Basic Concepts of Creating Shells . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .347 Adding Shell Features to Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .347 Using Replay to Examine Designs . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Assembly Drawing Views . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 425 Editing Assemblies. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 433 Editing External Subassemblies . . . . . . . . . . . . . . . . . . . . . . . . . . . . 433 Editing External Parts. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 434 Editing Assembly Constraints . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Creating Bills of Material . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .522 Customizing BOM Databases . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .523 Working with Part References. . . . . . . . . . . . . . . . . . . . . . . . . . . . . .525 Adding Balloons . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .527 Placing Parts Lists . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Chapter 21 Surfacing Wireframe Models . . . . . . . . . . . . . . . . . . . . . . . . . . . . 613 Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 614 Basic Concepts of Surfacing Wireframe Models . . . . . . . . . . . . . . . . . . . . 615 Discerning Design Intent . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 615 Identifying Logical Surface Areas. . . . . . . . . . . . . . . . . . . . . . . . . . .
Chapter 24 Calculating Stress on 3D Parts . . . . . . . . . . . . . . . . . . . . . . . . . . . 707 Key Terms . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .708 Tutorial at a Glance . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .709 Basic Concepts of 3D FEA . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .709 Using 3D FEA Calculations . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . .
Surface Modeling. . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . . 735 Surface Modeling ➤ AutoSurf Options . . . . . . . . . . . . . . . . . . . . . . 735 Surface Modeling ➤ Swept Surface . . . . . . . . . . . . . . . . . . . . . . . . . 736 Surface Modeling ➤ Loft U Surface . . . . . . . . . . . . . . . . . . . . . . . . . 736 Surface Modeling ➤ Blended Surface. . . . . . . . . . . . . . . . . . . . . . . . 736 Surface Modeling ➤ Flow Wires . . . . . . . . . . . . . . .
xiv
Part I Getting Started with Autodesk Mechanical Desktop ® ® Part I provides information for getting started with your Mechanical Desktop 6 software. It includes information to help in the transition from AutoCAD® and the migration of files from previous releases. It explains the user interface and the basics of modeling in the different work environments in Mechanical Desktop.
2 |
Welcome 1 In This Chapter This chapter provides an overview of the capabilities of Autodesk® Mechanical Desktop® 6 software. You learn ® about the transition from AutoCAD , data exchange, ■ About Mechanical Desktop ■ Making the transition from AutoCAD ■ Migrating files from previous releases and the migration of files from previous releases with the Mechanical Desktop Migration Assistance.
What is Autodesk Mechanical Desktop? Mechanical Desktop is a powerful and easy-to-use 3D parametric modeler used in mechanical design. Built on AutoCAD 2002, the Mechanical Desktop 6 design software package includes: ■ ■ ■ AutoCAD Mechanical 6 with the power pack (2D Parts and Calculations) Mechanical Desktop 6 with the power pack (Mechanical Desktop 6, 3D Parts and Calculations) AutoCAD 2002 When you start Mechanical Desktop 6, you have the option to run it with or without the power pack.
Making the Transition from AutoCAD Mechanical Desktop 6 is built on AutoCAD 2002 and uses many of the tools you may already be familiar with. Because Mechanical Desktop is a parametric modeling program, exercise care in using standard AutoCAD commands. In the sketching stage, you can use any AutoCAD command to create the geometry for your sketch. You can use AutoCAD drawing and editing tools to edit sketch geometry after it has been consumed by a feature.
To install the Mechanical Desktop Migration Assistance from your product CD 1 Hold down the SHIFT key while you insert the product CD into the CD-ROM drive. This prevents Setup from starting automatically. 2 In the file tree of the CD-ROM drive, navigate to the Migrate folder and click setup.exe. 3 Respond to the directions in the Mechanical Desktop Migration Assistance installation dialog boxes.
Modeling with Autodesk Mechanical Desktop ® ® 2 In This Chapter This chapter describes the basic concepts of mechanical design with Autodesk Mechanical Desktop software, ■ Mechanical Desktop basics ■ Mechanical Desktop work environments including fundamentals of parametric design. If you understand the underlying concepts in this chapter, you can become proficient in using the Mechanical Desktop software.
Mechanical Desktop Basics Mechanical Desktop is an integrated package of advanced 3D modeling tools and 2D drafting and drawing capabilities that helps you conceptualize, design, and document your mechanical products. You create models of 3D parts, not just 2D drawings. You use these 3D parts to create 2D drawings and 3D assemblies. 2D drawing 3D part Mechanical Desktop, a dimension-driven system, creates parametric models. Your model is defined in terms of the size, shape, and position of its features.
You create most features from sketches. Sketches can be extruded, revolved, lofted, or swept along a path to create features. sketch for revolved feature sketch for extruded feature You work in the Part Modeling environment to create single parts. In this environment, only one part can exist in a drawing. Additional parts become unconsumed toolbodies for the purpose of creating a combined part. Use part files to build a library of standardized parts.
Individual parts can be fit together to create subassemblies and assemblies. Assembly files contain more than one part. Parts are fit together using assembly constraints to define the positions of the individual parts that make up your final product. individual parts in an assembly file completed assembly For standard parts, you can define different versions using a spreadsheet.
You can create scenes to define how your design fits together. To better conceptualize the position of the parts in your assembly, you define scenes using explosion factors, tweaks, and trails that illustrate how your design is assembled. exploded scene You can create base, orthogonal, isometric, section, and detail views. To document your design, drawing views can be created from scenes, parts, or groups of selected objects. Any design changes are automatically updated in these drawing views.
12
The User Interface 3 In This Chapter When you start the Autodesk® Mechanical Desktop® 6 software, a page called the Today window is displayed. ■ The Today window ■ Work environments ■ Mechanical Desktop interface This chapter provides an overview of the options on the ■ Working in the Browser Today window to help manage your work, collaborate ■ Methods for issuing commands with others, and link to information on the Web.
Mechanical Desktop Today The first time you open the Mechanical Desktop 6 program, the Today window is displayed on top of the program interface, along with instructions about how to use it. The Today feature is a powerful tool that makes it easy to manage drawings, communicate with design teams, and link directly to design information. In the Today Window, you can expand the following options for access to the the services you require.
Mechanical Desktop Environments Mechanical Desktop has two working environments: Assembly Modeling and Part Modeling. Assembly Modeling Environment This is the environment Mechanical Desktop uses when you start the program or create a new file by using File ➤ New. Any number of parts and subassemblies can coexist in the same drawing. The advantages of the Assembly Modeling environment are ■ ■ ■ ■ More than one part can be created in the same drawing.
Part Modeling Environment To begin a new drawing in the Part Modeling environment, choose File ➤ New Part File. Only one part may exist in the drawing. If you add more parts, they automatically become unconsumed toolbodies. You use toolbodies to create complex combined parts. The advantages of the Part Modeling environment are ■ ■ ■ A library of standard parts can be created for use in assembly files. The interface is streamlined to allow only those commands available in a part file.
Mechanical Desktop Interface When you open a new or existing drawing in Mechanical Desktop 6, four toolbars and the Desktop Browser are displayed. ■ ■ ■ ■ ■ The Mechanical Main toolbar provides quick access to select commands from the AutoCAD Standard and the Object Properties toolbars, some Mechanical Desktop commands, and the Web. Icons are available for direct links to Mechanical Desktop Today window and Web tools such as, Point A, Streamline, RedSpark, MeetNow, Publish to Web, and eTransmit.
There are four main toolbars controlled by the Desktop Tools toolbar: Part Modeling, Assembly Modeling, Scene, and Drawing Layout. Part Modeling Assembly Modeling Scene Drawing Layout If you begin a drawing in the Part Modeling environment, the Desktop Tools toolbar changes to display three buttons that control the Part Modeling, Toolbody Modeling, and Drawing Layout toolbars.
AutoHide With AutoHide on, choose Collapse to minimize the Browser. When you move the cursor over and off of the Browser, it expands and collapses. Choose Right or Left to hide the Browser off a side of the screen. When you move your cursor to the corresponding edge of the screen, the Browser is displayed. Move the cursor off the Browser, and it is hidden again. To turn AutoHide off, in the Browser docking menu choose AutoHide ➤ Off. Hide Hides the Browser entirely.
You collapse levels by clicking the minus sign beside an object, or collapse the entire hierarchy by right-clicking the assembly name and choosing Collapse from the menu. When you start a new drawing in the Part Modeling environment, or open an existing part file, the Desktop Browser contains two tabs: Model and Drawing. In the Assembly Modeling environment, the Browser contains three tabs: Model, Scene, and Drawing.
The first icon, the Part filter, controls the display of assembly constraints attached to a part and its toolbodies. If the Part filter is selected, only the features of your part and its toolbodies are visible in the Browser. If it is not selected, assembly constraints are also visible. The second icon is the Assembly filter. If you select this filter, only assembly constraints that are attached to your part and its toolbodies are visible.
Using the Browser in Assembly Modeling In the Assembly Modeling environment, the Browser displays three tabs: Model, Scene, and Drawing. With these tabs, you can create multiple parts, assemblies, scenes, BOMs, and documents, and you can reorder assemblies. You can localize and externalize parts in the Browser without opening the Assembly Catalog.
Scene Mode in Assembly Modeling In Scene mode, three icons are displayed at the bottom of the Browser. The first icon accesses Desktop Options, where you can control the settings for scenes. The second icon accesses Desktop Visibility, where you can control the visibility of your parts, assemblies, and individual drawing objects. The last icon updates the active scene.
Issuing Commands You can issue commands in several ways: ■ ■ ■ ■ ■ ■ Select an option from a right-click menu in the Desktop Browser. Select an option from a right-click menu in the active screen area of your drawing. Select a toolbar icon. Select an option from a pull-down menu. Enter the command name on the command line. Use an abbreviation of the command, called an accelerator key, on the command line.
Using Context Menus in the Graphics Area In addition to the Browser menus, context-sensitive menus are available in the graphics area during the modeling process. When you start Mechanical Desktop, the Part menu is available in the graphics area. You can toggle between the Part and Assembly menus as you build your models. When you are in Scene mode, the Scene menu is available. In Drawing mode, you can toggle between the Drawing and Annotate menus.
Using Pull-down Menus To select a menu option, or access a submenu, hold down the left mouse button while you navigate through the menu. When you find the command you want to use, release the mouse button. You can also access menu commands by using the keyboard. Hold down ALT while selecting the underlined letter of the menu option. For example, to select AMPROFILE from the keyboard, press ALT, then P, S, P. Selecting Command Options from Dialog Boxes Many commands have options within dialog boxes.
Documentation and Support 4 In This Chapter This chapter provides an overview of the printed and ■ Mechanical Desktop print documentation online documentation provided with Autodesk® ® Mechanical Desktop 6. It guides you to resources for ■ Mechanical Desktop online documentation ■ Product Support Assistance in product learning, training, and support. Help ■ Mechanical Desktop learning Read this section so that any time you need product information, you will know where to locate it.
Printed and Online Manuals The extensive set of printed and online documentation provided with your purchase of Mechanical Desktop 6 software includes the printed Autodesk Mechanical Desktop 6 User’s Guide, AutoCAD Mechanical 6 User’s Guide, and the AutoCAD 2002 User’s Guide. The online AutoCAD Mechanical 6 and Mechanical Desktop 6 Installation Guide is provided on the product CD.
Chapter 2 Procedures to install, upgrade, authorize, and maintain the software for a single user, and information you need to know before you begin your installation. Chapter 3 Information for network administrators. Instructions for installing and configuring for a network environment. Chapter 4 Technical information about environment variables and performance enhancements to optimize performance of the software.
Mechanical Desktop Help The Help in Mechanical Desktop provides integrated information about AutoCAD Mechanical and Mechanical Desktop.
Product Support Assistance in Help When you need product support, refer to Support Assistance in the Help menu. Support Assistance ensures quick access to technical support information through an easy-to-use issue/solution format with self-help tools and a knowledge base.
Internet Resources Following are resources for information about Autodesk products and assistance with your Mechanical Desktop questions. ■ ■ ■ ■ ■ ■ Autodesk Web site: http://www.autodesk.com Mechanical Desktop home page at the Autodesk Web site: http://www.autodesk.com/mechdesktop AutoCAD Mechanical home page at the Autodesk Web site http://www.autodesk.com/autocadmech Mechanical Desktop discussion groups: http://www.autodesk.com/mechdesktop-discussion AutoCAD Mechanical discussion groups: http://www.
Part II Autodesk Mechanical Desktop Tutorials ® ® The tutorials in this section teach you how to use Mechanical Desktop 6, and provide a comprehensive overview of mechanical design. The lessons range from basic to advanced, and include step-by-step instructions and helpful illustrations. You learn how to create parts, surfaces, assemblies, table driven parts, and bills of material. You will also learn how to prepare your designs for final documentation.
34 |
Using the Tutorials 5 In This Chapter This Introduction presents information that is useful to know before you start performing the tutorials for ■ Finding the right tutorial ■ Accessing commands ■ Controlling the appearance of Autodesk® Mechanical Desktop®. It provides a summary of how the tutorials are structured, and the methods the Desktop Browser ■ Backing up tutorial files you can use to issue commands. You learn how to manipulate the position of the Browser to best suit your work space.
How the Tutorials are Organized Read the Key Terms and Basic Concepts sections at the beginning of each tutorial before you begin the step-by-step instructions. Understanding this information before you begin will help you learn. Key Terms Lists pertinent mechanical design terms and definitions for the lesson. Basic Concepts Gives you an overview of the design concepts you learn in the lesson. The tutorials begin with basic concepts and move toward more advanced design techniques.
Accessing Mechanical Desktop Commands Mechanical Desktop provides several methods to access commands and manage your design process. The following are samples of the access methods available to you: Browser Right-click the window background and choose New Part. Context Menu In the graphics area, right-click and choose Part ➤ New Part.
Positioning the Desktop Browser The Desktop Browser is a graphical interface that is useful in both creating and modifying your designs. You can do much of your work in the Browser as you proceed through the lessons in the tutorials. By default, the Browser is located on the left side of your screen. You may want to move, resize, or hide the Browser to suit your working conditions.
To hide and unhide the Browser To hide the Browser, right-click the gray area above the tabs and choose Hide. To unhide the Browser, choose View ➤ Display ➤ Desktop Browser. To move the Browser off the screen with Auto Hide, right-click the gray bar above the tabs and choose Auto Hide ➤ Left (or Right). After you move the Browser off the left or right side of the screen with Auto Hide, if you move your mouse to the corresponding edge of the screen, the Browser is displayed along that edge.
Backing up Tutorial Drawing Files For each tutorial, you use one or more of the master drawing files that contain the settings, example geometry, or parts for the lesson. These files are included with Mechanical Desktop. Before you begin the tutorials, back up these drawing files so you always have the originals available. Any mistakes you make while you are learning will not affect the master files. To back up tutorial drawing files 1 From the Windows Start menu, choose Programs ➤ Windows Explorer.
Creating Parametric Sketches 6 In This Chapter Autodesk® Mechanical Desktop® automates your design ■ Analyzing a design and creating a strategy for sketching and revision process using parametric geometry. Parametric geometry controls relationships among design elements and automatically updates models and ■ Text sketch profiles ■ Open profile sketches ■ Closed profile sketches ■ Path sketches drawings as they are refined.
Key Terms Term Definition 2D constraint Defines how a sketch can change shape or size. Geometric constraints control the shape and relationships among sketch lines and arcs. Dimensional constraints control the size of sketch geometry. closed loop A polyline entity, or group of lines and arcs that form a closed shape. Closed loops are used to create profile sketches.
Basic Concepts of Parametric Sketching You create, constrain, and edit sketches to define a ■ ■ ■ ■ ■ ■ Profile that governs the shape of your part or feature Location for a bend feature in a part design Path for your profile to follow Cut line to define section views Split line to split a face or part Break line to define breakout section views After you create a rough sketch with lines, polylines, arcs, circles, and ellipses to represent a feature, you solve the sketch.
Sketching Tips Some of these tips do not apply to this chapter, but you will see their usefulness when you use sketches to create complex parts. 44 | Tip Explanation Keep sketches simple It is easier to work with a single object than a multiple-object sketch. Combine simple sketches for complex shapes. Repeat simple shapes If a design has repeating elements, sketch one and then copy or array as needed. Define a sketching layer Specify a separate layer and color for sketching.
Creating Profile Sketches In Mechanical Desktop, there are three types of profile sketches: ■ ■ ■ Text-based profiles, used to create parametric 3D text-based shapes Open profile sketches, used to define features on parts Closed profile sketches, used to outline parts and features You can solve and apply parametric constraints and dimensions to all three of these profile sketch types. Creating Text Sketch Profiles A text sketch profile is a line of text displayed in a rectangular boundary.
Creating Open Profile Sketches You can create an open profile from single or multiple line segments, and solve it in the same way as you solve a closed profile. An open profile constructed with one line segment is used to define the location of a bend feature on a flat or cylindrical part model. To bend an entire part, you sketch the open profile over the entire part. If you sketch the open profile over a portion of a part, only that portion of the part bends.
In this section, you create three profile sketches. Open the file sketch1.dwg in the desktop\tutorial folder. This drawing file is blank but it contains the settings you need to create these profiles. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
To create a profile sketch from multiple objects 1 Use LINE to draw this shape, entering the points in the order shown. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Line.
Your sketch should look like this. 3 Create a profile sketch from the rough sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Profile. Select objects for sketch: Select the arc and the lines Select objects for sketch: Press ENTER As soon as the sketch is profiled, a part is created. The Browser contains a new icon labelled PART1_1. A profile icon is nested under the part icon.
When redrawing, Mechanical Desktop uses assumed constraints in the sketch. For example, lines that are nearly vertical are redrawn as vertical, and lines that are nearly horizontal are redrawn as horizontal. After the sketch is redrawn, a message on the command line tells you that Mechanical Desktop needs additional information: Solved under constrained sketch requiring 5 dimensions or constraints.
If your sketch does not contain the same constraints, redraw it to more closely resemble the illustrations in steps 1 and 2. Notice the letter F, located at the start point of line 0. It indicates that a fix constraint has been applied to that point. When Mechanical Desktop solves a sketch, it applies a fix constraint to the start point of the first segment of your sketch. This point serves as an anchor for the sketch as you make changes.
To create a new part definition 1 Use the context menu to initiate a new part definition. Context Menu In the graphics area, right-click and choose Part ➤ New Part. 2 Respond to the prompts as follows: Select an object or enter new part name : Press ENTER NOTE The command method you use determines which prompts appear. A new part definition is created in the drawing and displayed in the Browser. The new part automatically becomes the active part.
5 1 4 6 2 3 2 Following the prompts, switch to Arc to create the arc segment, then switch back to Line. Switch to Close to finish the sketch.
All lines were redrawn as horizontal or vertical except one. L1 remains angled because the angle of the line exceeds the setting for angular tolerance. By default, this rule makes a line horizontal or vertical if the angle is within 4 degrees of horizontal or vertical. L1 You can modify this and other sketch tolerance settings to adjust the precision of your sketch analysis. 4 Change the angular tolerance setting. Browser Click the Options button below the window.
6 Reprofile the sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Profile. NOTE You cannot use Single Profile to reprofile a sketch. Select objects for sketch: Use a crossing window to specify the sketch Select objects for sketch: Press ENTER L1 If your sketch shows line L1 unchanged, the angle was greater than 10 degrees. You need to edit or redraw the shape and append the sketch.
Using Nested Loops You can select more than one closed loop to create a profile sketch. A closed loop must encompass the nested loops. They cannot overlap, intersect, or touch. With nested loops you can easily create complex profile sketches. To create a profile sketch using nested loops 1 Use AMNEW to create a new part definition. Context Menu In the graphics area, right-click and choose Part ➤ New Part. 2 Accept the default part name on the command line. The Browser now contains a third part.
5 Profile the sketch, following the prompts to select the objects with a crossing window. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Profile. Select objects for sketch: Specify a point to the right of the sketch (1) Specify opposite corner: Specify a second point (2) 5 found Select objects for sketch: Press ENTER 1 2 Mechanical Desktop calculates the number of dimensions or constraints required to fully constrain the profile.
Creating Path Sketches Path sketches can be both two dimensional and three dimensional. Like open profile sketches, they can be open shapes. In this exercise, you create only the path sketches, but not the profiles that would sweep along the paths. Creating 2D Path Sketches A 2D path sketch serves as a trajectory for a swept feature. You create a swept feature by defining a path and then a profile sketch of a cross section. Then, you sweep the profile along the path.
To create a 2D path sketch 1 Create a new part definition. Context Menu In the graphics area, right-click and choose Part ➤ New Part. 2 Press ENTER on the command line to accept the default part name. 3 Pan the drawing so you have room to create the next sketch. Context Menu In the graphics area, right-click and choose Pan. 4 Use PLINE to draw the rough sketch as a continuous shape, responding to the prompts to specify the points in the following illustration.
5 Use AM2DPATH to convert the rough sketch to a path sketch, following the prompts. Context Menu Select objects: Select objects: In the graphics area, right-click and choose Sketch Solving ➤ 2D Path. Specify the polyline shape Press ENTER At the prompt for the start point of the path, you select the point where the path begins. This determines the direction to sweep the profile of the cross section.
A work point is automatically placed at the start point of the path. The Browser displays both a 2DPath icon and a work point icon nested below the part definition. 6 Use AMSHOWCON to display the existing constraints, responding to the prompt. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Show Constraints. Enter an option [All/Select/Next/eXit] : Enter a The start point of the path is fixed. Both lines are vertical and are tangent to the endpoints of the arc.
Creating 3D Path Sketches 3D path sketches are used to create ■ ■ ■ ■ A 3D path from existing part edges A helical path The centerline of a 3D pipe A 3D spline path 3D paths are used to create swept features that are not limited to one plane. See chapter 8, “Creating Sketched Features,” to learn more about sweeping features along a 3D path. Open the file sketch2.dwg in the desktop\tutorial folder. The drawing contains four part definitions and the geometry you need to create the 3D paths.
Before you can work on a part, it must be active. Activate PART1_1, responding to the prompts. Context Menu In the graphics area, right-click and choose Part ➤ Activate Part. Select part to activate or [?] : Enter PART1_1 PART1_1 is activated, and highlighted in the Browser. Use Pan to center PART1_1 on your screen. Context Menu In the graphics area, right-click and choose Pan. PART1_1 contains an extruded part.
2 Continue on the command line to place the work plane. Plane=Parametric Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER The path is created, and a work point is located at the start point. A work plane is placed normal to the start of the path so you can sketch the profile for the sweep feature. In the Browser, the new geometry is nested below the extrusion and fillets in PART1_1. Save your file.
Creating a 3D Helical Path A 3D helical path is used for a special type of swept feature. Helical sweeps are used to create threads, springs, and coils. You create a 3D helical path from an existing work axis, cylindrical face, or cylindrical edge. 3D path profile sketch 3D helical sweep When you create a 3D helical path, you can specify whether a work plane is also created. The work plane can be normal to the path, at the center of the path, or along the work axis.
To create a 3D helical path 3 Use AM3DPATH to define the 3D helical path, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ 3D Helix Path. Enter path type [Helical/Spline/Edge/Pipe] : Enter h Select work axis, circular edge, or circular face for helical center: Select the work axis (1) The command method you use determines the prompts that are displayed.
The 3D helix path is created. A work point is placed at the beginning of the path. You can also specify that a work plane is placed normal to the start point of the 3D path, at the center of the path, or along the work axis. This option makes it easier for you to create the sketch geometry for the profile you sweep along the path. Save your file. Creating a 3D Pipe Path A 3D pipe path is used to sweep a feature along a three-dimensional path containing line and arc segments or filleted polylines.
Use Pan to center PART3_1 on your screen. PART3_1 contains an unsolved sketch of line segments and arcs. To create a 3D pipe path 1 Use AM3DPATH to define the 3D pipe path, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ 3D Pipe Path.
2 In the 3D Pipe Path dialog box, examine the vertices and angles of the path. Verify that Create Work Plane is selected. NOTE Your numbers might not match the illustration above. Choose OK to exit the dialog box. 3 Place the work plane, following the prompts. Plane=Parametric Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER The Desktop Browser now contains a 3D Pipe icon, a work plane, and a work point nested below the PART3_1 definition. Save your file.
Creating a 3D Spline Path In this type of path, you sweep a feature along a 3D spline created with fit points or control points. Working in one integrated dialog box, you can modify any fit point or control point in a 3D spline path, and you can convert fit points to control points, and control points to fit points. In this exercise, you work with a fit point spline. 3D spline path and profile sketch 3D sweep along spline path Before you begin, activate PART4_1 from the Browser.
2 In the 3D Spline Path dialog box, examine the vertices of the spline, and verify that Create Work Plane is selected. NOTE Your numbers might not match the illustration above. Choose OK to exit the dialog box. 3 Create the work plane, responding to the prompts. Plane=Parametric Select edge to align X axis or [Flip/Rotate/Origin] : Press ENTER The path is created, and a work point is located at the start point.
Creating Cut Line Sketches When you create drawing views, you might want to depict a cut path across a part for offset, cross-section views. After you have extruded or revolved a profile sketch to create a feature, you can return to an original sketch and draw the cut line across the features you want to include in the cross section. There are two types of cut line sketches: offset and aligned. An offset cut line sketch is a two-dimensional line constructed from orthogonal segments.
In the following exercise, after you create a cut line sketch on these models, the resulting cross-section drawing views can be generated in Drawing mode. A cut line sketch is needed when you want to define a custom cross-section view only, but not for a half or full cross-section view. Open the file sketch3.dwg in the desktop\tutorial folder. The drawing contains two parts. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake.
To create an offset cut line sketch 1 Use PLINE to sketch through the center of the holes on the square part. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Polyline. Next, analyze the cut line sketch according to internal sketching rules. 2 Use AMCUTLINE to solve the cut line, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Cut Line.
As with the other sketches you created, a message tells you how many dimensions and constraints are needed to fully solve the sketch. In this case, you need five dimensions or constraints to complete the definition of the sketch: three to define the shape of the sketch, and two to constrain it to the part. When you create a cross-section drawing view, this sketch defines the path of the cut plane.
To create an aligned cut line sketch 1 Use PLINE to sketch through the centers of two of the holes on the circular part. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Polyline. 2 Define a cut line on your sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Cut Line.
Creating Split Line Sketches A molded part or casting usually requires two or more shapes to define the part. To make a mold or a cast, you create the shape of your part and then apply a split line to split the part into two or more pieces. You may also need to apply a small draft angle to the faces of your part so that your part can be easily removed from the mold. Split lines can be as simple as a planar intersection with your part, or as complex as a 3D polyline, or spline, along planar or curved faces.
To create a split line 1 Expand the Browser hierarchy of SKETCH4 and PART1_1. The part consists of an extrusion, three fillets, and a shell feature. Next, you create a sketch plane on the outside right face of the part. 2 In the right viewport, define a new sketch plane, responding to the prompts. Context Menu In the graphics area, right-click and choose New Sketch Plane.
3 In the left viewport, use PLINE to sketch the split line. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Polyline. 4 Use AMSPLITLINE to create a split line from your sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Split Line.
Creating Break Line Sketches When you want to document complex assemblies, it is not always easy to display parts and subassemblies that are hidden by other parts in your drawing views. By creating a break line sketch, you can specify what part of your model will be cut away in a breakout drawing view so that you can illustrate the parts behind it. break line path breakout drawing view Open the file sketch4a.dwg in the desktop\tutorial folder.
To create a break line 1 Use AMBREAKLINE to define the break line sketch, following the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Break Line. Select objects for sketch: Specify the sketch (1) Select objects for sketch: Press ENTER 1 The break line is created. The Browser contains a break line icon nested below the work plane. Save your file.
82
Constraining Sketches 7 In This Chapter When you solve a sketch in Autodesk® Mechanical ■ Creating a strategy for constraining and dimensioning Desktop®, geometric constraints are applied in accordance with internal rules. To fully constrain the sketch, you apply the remaining parametric dimensions and geometric constraints that are necessary to meet your design goals.
Key Terms Term Definition 2D constraint Defines how a sketch can change shape or size. Geometric constraints control the shape and relationships among sketch lines and arcs. Dimensional constraints control the size of sketch geometry. degree of freedom In part modeling, determines how a geometric object such as a line, arc, or circle can change shape or size. For example, a circle has two degrees of freedom, center and radius. When these values are known, degrees of freedom are said to be eliminated.
Basic Concepts of Creating Constraints A sketch needs geometric and dimensional constraints to define its shape and size. These constraints reduce the degrees of freedom among the elements of a sketch and control every aspect of its final shape. When you solve a sketch, Mechanical Desktop applies some geometric constraints. In general, use the automatically applied constraints to stabilize the sketch shape.
Constraining Tips Tip Explanation Determine sketch dependencies Analyze the design to determine how sketch elements interrelate; then decide which geometric constraints are needed. Analyze automatically applied constraints Determine the degrees of freedom not resolved by automatic constraints. Decide if any automatic constraints need to be deleted in order to constrain elements as you require. Use only needed constraints Replace constraints as needed to define shape.
The ways a sketch can change size or shape are called degrees of freedom. For example, a circle has two degrees of freedom—the location of its center and its radius. If the center and radius are defined, the circle is fully constrained and those values can be maintained. radius center Similarly, an arc has four degrees of freedom—center, radius, and the endpoints of the arc segment. endpoint radius center endpoint The degrees of freedom you define correspond to how fully the sketch is constrained.
Applying Geometric Constraints When constraining a sketch, begin by defining its overall shape before defining its size. Geometric constraints specify the orientation and relationship of the geometric elements. For example ■ ■ Constraints that specify orientation indicate whether an element is horizontal or vertical.
As you apply geometric constraints, you should continue to analyze your sketch, reviewing and replacing constraints. In the next exercise, you gain experience with constraining techniques by analyzing and then modifying geometric constraints to reshape the sketch. Open the file sketch5.dwg in the desktop\tutorial folder. Use the before-andafter sketches below to determine what changes you must make. Then change the constraints and see the results of your analysis.
Showing Constraint Symbols You can change the parametric relationships of the lines by modifying geometric or dimensional constraints. Because geometric constraints control the overall shape of the sketch, you cannot safely make any changes until you know the current geometric constraints. Therefore, the next step is to show the symbols. To show constraint symbols 1 Use AMSHOWCON to display constraint symbols, responding to the prompt.
Similarly, the constraint symbols (P2, P4, and P6) show that line 0 is parallel to lines 2, 4 and 6. 2 Hide the constraint symbols. Enter an option [All/Select/Next/eXit] : Press ENTER Replacing Constraints After you delete the unwanted constraints, you can add constraints to reshape the sketch. In this exercise, you delete the parallel constraints that control the inner and outer angled lines in the sketch and replace them with vertical constraints.
2 Use AMADDCON to add vertical constraints to the two inner angled lines, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Vertical. Valid selection(s): line, ellipse or spline segment Select object to be reoriented: Specify line (3) Solved under constrained sketch requiring 2 dimensions or constraints.
3 Use AMPARDIM to add an angular dimension, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Select near the middle of line (1) Select second object or place dimension: Select near the middle of line (2) Specify dimension placement: Place the dimension (3) Enter dimension value or [Undo/Placement point] <75>: Enter 105 Solved fully constrained sketch.
Applying Dimension Constraints It is good practice to stabilize the shape of a sketch with geometric constraints before you specify size with dimensional constraints. Dimensions specify the length, radius, or rotation angle of geometric elements in the sketch. Unlike geometric constraints, dimensions are parametric; changing their values causes the geometry to change. Dimensions can be shown as numeric constants or as equations. Although you can use them interchangeably, they each have specific uses.
In this case, the height of the sketch must maintain the same proportion to the length, even if you change dimensions later. In an equation, you can state the height relative to the length. The dimension for the vertical line is defined as an equation of d1 = d0/.875 where d1 is the parameter name for the vertical line and d0 is the parameter name for one of the horizontal lines. The d variables in the equations are parameter names assigned by Mechanical Desktop when you define the parameters.
Creating Profile Sketches First, convert the unconstrained sketch to a profile sketch before you add dimensions. Then examine the default geometric constraints. To create a profile from a sketch and examine constraints 1 Use AMPROFILE to create a profile from the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile.
Mechanical Desktop recalculates the sketch and displays the constraints. ■ ■ ■ A fix constraint is added to the start point of the first line of the sketch. This point is anchored and will not move when changes are made to the sketch constraints. Nearly horizontal and vertical lines have been assigned horizontal (H) and vertical (V) constraints. Nearly vertical lines are assumed to be parallel (P) to one another.
To add a dimension to a profile 1 Use AMPARDIM to add dimensions to your profile, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Specify the line (1) Select second object or place dimension: Place the dimension (2) Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <1.9606>: Enter 2 Solved under constrained sketch requiring 5 dimensions or constraints.
Now that the default constraints and larger dimensions have stabilized the sketch shape and size, you can begin to make changes to the sketch. To practice changing and updating the sketch, you add fillets to the two legs of the sketch. To add a fillet to a sketch 1 Use AMFILLET to apply a fillet, entering the points in the order shown. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Fillet. Current settings: Mode = TRIM, Radius = 0.
Before you continue defining your sketch, erase the horizontal line and the vertical line joining the endpoints of the new arcs. 3 Erase the two lines. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Erase. Your drawing should look like this. Because you have changed the sketch, you must re-solve it before you can use it to create a feature. Appending Sketches By adding the fillets and removing the lines, you have changed the sketch geometry.
To append a profile sketch and re-examine geometric constraints 1 Expand the hierarchy of PART1_1. 2 Use AMRSOLVESK to append the existing fillets, responding to the prompts. Context Menu In the graphics area, right-click and choose Append Sketch. Select geometry to append to sketch: Specify the first arc Select geometry to append to sketch: Specify the second arc Select geometry to append to sketch: Press ENTER Redefining existing sketch.
For this exercise, do not delete any constraints because the tangent constraints do not adversely affect the dimensioning scheme. Now that you have recreated the profile sketch, you can continue to add geometric constraints and dimensions to the sketch, starting with a radial constraint to the two arcs. Depending on how you drew your sketch, your default dimension values may differ from those in this exercise.
2 Use AMPARDIM to dimension the leftmost arc, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Specify the lower arc Select second object or place dimension: Place the dimension Enter dimension value or [Undo/Diameter/Ordinate/Placement point] <0.3687>: Enter .4 Solved under constrained sketch requiring 2 dimensions or constraints.
The dimensions are placed. Your sketch should be fully constrained.. Save your file. Modifying Dimensions Because your design changes during development, you must be able to delete or modify dimension values. Mechanical Desktop parametric commands ensure that relationships among geometric elements remain intact. To finish the sketch, change the dimension of the top horizontal line and the angular dimension. To change a dimension 1 Use AMMODDIM to modify the dimensions, responding to the prompts.
Your finished sketch should now look like this. Save your file. Using Construction Geometry Construction geometry can minimize the number of constraints and dimensions needed in a sketch and offers more ways to control sketch features. Construction geometry works well for sketches that are symmetrical or have geometric consistencies. Some examples are sketches that have geometry lying on a radius, a straight line, or at an angle to other geometry.
To create a single profile sketch 1 Use PLINE to draw the rough sketch. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Polyline. 2 Use AMSOLVE to solve the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. The polyline is automatically selected. Mechanical Desktop applies constraints according to how you sketch and then reports that the sketch needs six or more additional constraints.
To create a construction line 1 Create a construction line. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Construction Line. 2 Draw the line diagonally across the sketch. Mechanical Desktop draws the line on a new layer called AM_CON. The line is yellow and drawn with the HIDDEN linetype. Because the linetype is different from the one used to draw the sketch, the line is considered construction geometry. It is used only in this sketch. 3 Use AMRSOLVESK to append the profile.
To add a project constraint 1 Use AMADDCON to add the project constraints, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Project.
Adding Parametric Dimensions To fully define the sketch, dimension one of the risers and apply a slope angle for the construction line. Each step is equal in height, so you can add equal length constraints to the remaining steps later. To add a parametric dimension 1 Use AMPARDIM to dimension the slope angle, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
To add an equal length constraint 1 Use AMADDCON to add an equal length constraint, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Equal Length. Valid selections: line or spline segment Select object to be resized: Specify the second riser (2) Valid selections: line or spline segment Select object to base size on: Specify the dimensioned riser (1) Solved under constrained sketch requiring 1 dimensions or constraints.
Constraining Path Sketches Construction geometry helps you constrain sketches that may be difficult to constrain with only the geometry of the sketch shape. In this exercise, you create a path sketch, add a construction line, and constrain the sketch to the line. Before you begin this exercise, create a new part definition for the sketch. To create a new part definition 1 Use AMNEW to create a new part definition. Context Menu In the graphics area, right-click and choose Part ➤ New Part.
2 Use AM2DPATH to create a 2D path from your sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ 2D Path. Select objects: Specify the polyline Select objects: Press ENTER Specify the start point of the path: Specify one of the ends of the path Solved under constrained sketch requiring 10 dimensions or constraints. Create a profile plane perpendicular to the path? [Yes/No] : Enter n You can use either end for the start point.
To check for and add missing constraints 1 Use AMSHOWCON to check for constraints that are still needed. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Show Constraints. 2 Display all the constraints and press ENTER to exit the command. 3 Use AMADDCON to add constraints and dimensions to the sketch, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
5 Constrain all the arcs with the same radius as the one you just dimensioned, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Radius. Valid selections: arc or circle Select object to be resized: Specify the lower left arc Valid selections: arc or circle Select object radius is based on: Specify the arc with the radial dimension Solved under constrained sketch requiring 3 dimensions or constraints.
Controlling Tangency A single piece of construction geometry can manage the size and shape of entire sketches. Circles and arcs are particularly useful for constraining the perimeter shapes of nuts, knobs, multisided profiles, and common polygons. In this exercise, you create a triangular sketch and then constrain the sides of the triangle and the internal angles to remain equal. In this manner, you could form the basis for a family of parts in which the only variable is a single diameter dimension.
3 Use AMPROFILE to turn the sketch into a profile sketch, making sure to select both the polyline and the circle. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Profile. At this point, the circle may be tangent to some or all of the sides of the triangle. 4 Use AMADDCON to add Tangent constraints to the sketch, following the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Tangent.
To add a dimension to an angle 1 Use AMPARDIM to apply angular dimensions to the triangle, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
To add a dimension to a circle 1 Add a dimension to the diameter of the construction circle, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Specify a point on the circle Select second object or place dimension: Specify a point outside of the triangle Enter dimension value or [Undo/Radius/Ordinate/Placement point] <3.1541>: Enter 10 Solved fully constrained sketch.
All sides remain equal in length and tangent to the circle, and the bottom of the triangle remains horizontal. If you used this sketch as a base feature of a part, you could change the overall size of the part simply by changing the diameter of the construction circle. This technique could be applied to more complex geometry such as pentagons, octagons, and odd-shaped polygons. These shapes can form the base feature for a family of nuts, bolts, fittings, and so on. Try these types of sketches on your own.
120
Creating Sketched Features 8 In This Chapter Features are the parametric building blocks of parts. By creating and adding features you define the shape of ■ Extruded features ■ Loft features ■ Revolved features your part. Because features are parametric, any changes ■ Face splits to them are automatically reflected when the part is ■ Sweep features updated. In Autodesk® Mechanical Desktop®, there are three types of features—sketched, work and placed.
Key Terms Term Definition base feature The first feature you create. As the basic element of your part, it represents its simplest shape. All geometry you create for a part depends on the base feature. Boolean modeling A solid modeling technique in which two solids are combined to form one resulting solid. Boolean operations include cut, join, and intersect. Cut subtracts the volume of one solid from the other. Join unites two solid volumes. Intersect leaves only the volume shared by the two solids.
Basic Concepts of Sketched Features Features are the building blocks you use to create and shape a part. Because they are fully parametric, they can easily be modified at any time. The first feature in a part is called the base feature. As you add more features, they can be combined with the base feature or each other to create your part. Boolean operations, such as cut, join, and intersect, can be used to combine features after a base feature has been created.
The drawing file includes fifteen parts which contain the geometry you need to create the sketched features in this section. NOTE For clarity, the work features are not shown. First, you create an extruded feature. Creating Extruded Features Extrusions are the most common sketched features. An extruded feature can be created from a closed profile, an open profile, or a text-based profile.
Clear the visibility of the other parts, and display the dimensions and work features of the active part. To turn off the visibility of multiple parts Browser Select EXTRUDERIB_1, then hold down SHIFT as you select BEND_1. Right-click the selected block and choose Visible. NOTE Because most of the parts do not contain features yet, you cannot use the toolbutton, menu, or command methods to make the part instances invisible. Click the plus sign in front of EXTRUDE_1 to expand the hierarchy.
To zoom in to a part Browser Right-click EXTRUDE_1, and choose Zoom to. The EXTRUDE_1 part is positioned on your screen. To create an extruded feature 1 Use AMEXTRUDE to create an extruded feature from Profile1. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Distance: Enter 0.5 Termination: Type: Blind The image tile indicates the direction of the extrusion. Choose OK.
The profile is extruded perpendicular to the plane of the profile. Next, you create and constrain another profile, and extrude it to cut material from the base feature. To create a profile sketch 1 Change to the top view of your part. Desktop Menu View ➤ 3D Views ➤ Top 2 Use RECTANGLE to sketch a rectangle as shown in the following illustration, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Rectangle.
3 Use AMRSOLVESK to solve the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. The command line indicates the number of constraints required to fully constrain the profile. Solved underconstrained sketch requiring 4 dimensions or constraints. Before you extrude the profile, fully constrain it by adding four dimensional constraints. To constrain a sketch 1 Use AMPARDIM to add parametric dimensions to fully constrain the sketch, responding to the prompts.
2 Continue creating the parametric dimensions. Select first object: Specify the right edge (5) Select second object or place dimension: Place the dimension (6) Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.4500>: Enter .5 Solved underconstrained sketch requiring 1 dimensions or constraints.
To add an extruded feature to a part 1 Change to an isometric view. Desktop Menu View ➤ 3D Views ➤ Front Right Isometric 2 Extrude the profile. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. 3 In the Extrusion dialog box, specify the following: Operation: Cut Distance: Enter 0.25 Termination: Blind 4 Choose OK to exit the dialog box. Your part should look like this. Save your file.
To modify a consumed profile 1 Expand ExtrusionBlind2 in the Browser. 2 Edit the dimensions of the profile used to define the shape of the extrusion, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit. Enter an option [Sketch/surfCut/Toolbody/select Feature]
4 Use AMUPDATE to update your part. Context Menu In the graphics area, right-click and choose Update Part. The part now reflects the changes to the profile that controls the shape of the extrusion you used to cut material from the part. Next, modify the extrusion feature to change the depth of the cut. To modify a feature 1 Select the cut extrusion to modify, responding to the prompt. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit.
Your part should look like this. Save your file. Extruding Open Profiles You extrude open profiles to create rib features and thin features. For more information about sketching open profiles, see “Creating Open Profile Sketches” on page 46. Creating Rib Features To create a rib feature on a part model, you sketch an open profile to shape the rib, define the thickness of the rib, and extrude it to part surfaces.
In this exercise, you extrude a rib feature to two perpendicular walls of a part. Turn off visibility for EXTRUDE_1, and make EXTRUDERIB_1 visible. Browser Right-click EXTRUDE_1 and choose Visible. Then rightclick EXTRUDERIB_1 and choose Visible. Activate EXTRUDERIB_1 and position it on your screen. Browser Double-click EXTRUDERIB_1. Then right-click EXTRUDERIB_1 and choose Zoom to. In the previous exercise, you made the work feature layer visible.
3 Use AMPROFILE to solve the sketch, responding to the prompt. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. Select part edge to close the profile : Press ENTER An icon for the open profile is displayed in the Browser. 4 Use AMPARDIM to add an angular dimension between the lower wall and the lower section of the rib, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
In the Rib dialog box, specify: Type: Midplane Thickness: .05 Choose OK. 6 Use 3DORBIT to rotate your part so you can see the rib feature. Your part should look like this. Creating Thin Features To create a thin feature, you sketch an open profile and extrude it to part surfaces. When you extrude an open profile, the Extrusion dialog box includes the options for defining a thin wall feature.
In this exercise, you create a thin wall in a shell. In the Browser, turn off visibility for EXTRUDERIB_1, and make EXTRUDETHIN_1 visible. Browser Right-click EXTRUDERIB_1 and choose Visible. Then right-click EXTRUDETHIN_1 and choose Visible. Activate EXTRUDETHIN_1 and position it on your screen. Browser Double-click EXTRUDETHIN_1. Then right-click EXTRUDETHIN_1 and choose Zoom to. To create a thin feature 1 Use AMWORKPLN to create a work plane for the profile sketch.
3 Use LINE to sketch the thin feature. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Line Specify first point: Specify the start point of the line (1) Specify next point or [Undo]: Specify the end point of the line (2) and press ENTER 1 2 NOTE Turn OSNAP off so that you will not snap to the back face when you pick. 4 Use AMRSOLVESK to solve the sketch, responding to the prompt. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile.
Choose OK. 7 Respond to the prompt: Select Face: Select the back face of the shell and press ENTER Enter an option [Next/Accept] : Press ENTER Your part should look like this. A thin wall is created with equal thickness on each side of the profile. In the Browser, an icon is displayed for the thin extrusion. NOTE When you extrude an open profile, the Extrusion dialog box contains options for defining a thin feature.
Creating Emboss Features Emboss features are text sketch profiles extruded on part models. A text sketch profile is one line of text displayed in a rectangular boundary. To create a text sketch profile, you define a font and a style, and enter one line of text. Then you place the text on an active sketch plane on your part, and extrude it to emboss the surface of your part with the text. Delete the thin extrusion from your shell part. Browser Right-Click ThinExtrusionToFace1 and choose Delete.
In the Text Sketch dialog box, specify: True Type Font: Sans Serif Style: Regular Text: Enter Autodesk Choose OK. 4 Define a location for the text sketch with a rotation angle of 15, responding to the prompts.
As you move the cursor, the rectangular border adjusts to accommodate the size of the text. In the Browser, an icon is displayed for the text sketch. You can change the parametric dimension for the height, and you can control the placement of the text object with typical 2D constraints and parametric dimensions between the rectangular boundary and other edges or features on your part. After the text sketch is positioned on the part, you can extrude it. 5 Use AMEXTRUDE to extrude the text sketch.
Editing Emboss Features You can edit the text in an emboss feature using the Text Sketch dialog box before the text sketch is consumed. After a text sketch is consumed by a feature, you can edit the feature dimensions or the sketch font and style. Creating Loft Features You create loft features by defining a series of cross sections through which the feature is blended. Lofts may be linear or cubic. Both types can be created with existing part faces as the start and end sections.
To create a linear loft 1 Expand LOFT1_1 in the Browser. Minimize EXTRUDE_1. 2 Zoom in to LOFT1_1. Desktop Menu View ➤ Zoom ➤ All The LOFT1 part contains two planar sections you use to create a linear lofted feature. 3 Create the loft feature, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Loft.
5 Choose OK to exit the Loft dialog box. Mechanical Desktop® calculates and displays the loft feature. Save your file. Next, you create a cubic loft blended through three planar sections. Creating Cubic Lofts A cubic loft is created by a gradual blend between two or more planar sections. Before the loft begins blending with the next section, you can control the tangency and the take-off angle at the start and end sections, and the distance the loft follows the tangent or angle options.
LOFT2 contains three profiles defining the sections you use for the loft feature. 5 Create the loft, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Loft.
To change the number of isolines 1 Modify the ISOLINES system variable. Command ISOLINES New value for ISOLINES <4>: Enter 6 2 Regenerate your drawing. Desktop Menu View ➤ Regen Mechanical Desktop regenerates the drawing and displays the loft using more isolines. NOTE A higher value for ISOLINES increases the time it takes to recalculate a part. In general, keep ISOLINES at its default value (4). 3 Reset the value of ISOLINES to its default setting.
To create a cubic loft from an existing face 1 Make LOFT3_1 visible. 2 Activate LOFT3_1. 3 Make LOFT2_1 invisible. 4 Zoom in to LOFT3_1. LOFT3 contains an existing extrusion and two profiles parametrically constrained to it. NOTE For clarity, the parametric dimensions are not shown. 5 Select the profiles to use for the cubic loft, following the prompts, and join the loft to the existing extrusion. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Loft.
6 In the Loft dialog box, specify: Operation: Join Type: Cubic Choose OK to exit the Loft dialog box. Your drawing should look like this. Save your file. Editing Loft Features You edit loft features the same way extruded features are edited—change the profiles or modify the loft feature itself. Try editing the loft features you created in this section.
Creating Revolved Features You create revolved features by revolving a closed profile about an axis. The axis may be a work axis or a part edge. To create a revolved feature about a work axis 1 Make REVOLVE_1 visible. 2 Activate REVOLVE_1. 3 Expand REVOLVE_1 and make Work Axis1 visible. 4 Make LOFT3_1 invisible. 5 Zoom in to REVOLVE_1. REVOLVE_1 contains a profile parametrically constrained to a work axis. work axis NOTE For clarity, the parametric dimensions are not shown. 6 Create a revolved feature.
Choose OK. Mechanical Desktop calculates and displays the feature. Save your file. Editing Revolved Features Edit a revolved feature by making changes to the profile, or by modifying the feature itself (like editing extruded and lofted features). Try editing your revolved feature following the procedures for editing extruded features you learned earlier in this tutorial.
Creating Face Splits Use face splits to split existing part faces. They can be created with ■ ■ ■ An existing part face A work plane A split line First, use one of the part’s existing faces to split a face. To split a face using an existing part face 1 Make FSPLIT_1 visible. 2 Activate FSPLIT_1. 3 Make REVOLVE_1 invisible. 4 Zoom in to FSPLIT_1. FSPLIT_1 contains a part, a work plane, and a split line. work plane split line NOTE For clarity, the parametric dimensions are not shown.
1 2 Mechanical Desktop splits the back face into two faces. Next, split a face using a work plane. To split a face using a work plane 1 Create the face split, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Face Split.
Your drawing should look like this. Now split the front face using the split line sketch. To split a face using a split line 1 Make Work Plane2 invisible. 2 Create the face split, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Face Split.
When you choose the Project option, Mechanical Desktop automatically looks for an unconsumed split line. If more than one split line exists, you are prompted to select the split line for the face split. Mechanical Desktop displays the new face split. The Browser contains three face split features. Save your file. Editing Face Splits Face splits created from an existing planar face can be edited by modifying the position of the face on the part.
Creating 2D Sweep Features You create a 2D sweep feature by sweeping a profile along a path that lies on a 2D plane. The feature may be the base feature of your part, or you can use Boolean operations to cut, intersect, split, or join the feature to your part. To create a 2D sweep 1 Make SWEEP1_1 visible. 2 Activate SWEEP1_1. 3 Make FSPLIT_1 invisible. 4 Zoom in to SWEEP1_1. SWEEP1_1 contains a solved profile constrained to the start of a 2D path.
Your drawing should look like this. NOTE Increase the value of ISOLINES for a more accurate display of the sweep. Save your file. Creating 3D Sweep Features With Mechanical Desktop, you can also sweep profiles along a variety of 3D paths.
SWEEP2_1 contains a cylinder and a helical path. A solved profile is constrained to the start of the path. 5 Create the 3D helical sweep. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Sweep. 6 In the Sweep Feature dialog box, choose OK to accept the settings. You can create a cut, join, intersection, or split feature. These options are available because there is a base feature in the part definition. Choose OK to exit the dialog box.
To create a spiral 3D sweep 1 Make SWEEP3_1 visible. 2 Activate SWEEP3_1. 3 Make SWEEP2_1 invisible. 4 Zoom in to SWEEP3_1. SWEEP3_1 contains a spiral helical path and a solved profile constrained to the start of the path. The spiral path is elliptical. 5 Create the 3D sweep. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Sweep. 6 In the Sweep Feature dialog box, choose OK to accept the settings. Your drawing should look like this. Save your file.
To create a sweep from a 3D edge path 1 Make SWEEP4_1 visible. 2 Activate SWEEP4_1. 3 Make SWEEP3_1 invisible. 4 Zoom in to SWEEP4_1. SWEEP4_1 contains a 3D edge path and a solved profile constrained to the start of the path. 5 Create the sweep. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Sweep. 6 In the Sweep Feature dialog box, choose OK to accept the settings. Your drawing should look like this. Save your file.
To create a sweep from a 3D pipe path 1 Make SWEEP5_1 visible. 2 Activate SWEEP5_1. 3 Make SWEEP4_1 invisible. 4 Zoom in to SWEEP5_1. SWEEP5_1 contains a 3D pipe path and a solved profile constrained to the start of the path. 5 Create the sweep. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Sweep. 6 In the Sweep dialog box, choose OK to accept the settings. Your drawing should look like this. Save your file.
To create a sweep from a 3D spline path 1 Make SWEEP6_1 visible. 2 Activate SWEEP6_1. 3 Make SWEEP5_1 invisible. 4 Zoom in to SWEEP6_1. SWEEP6_1 contains a 3D spline path and a solved profile constrained to the start of the path. 5 Create the sweep. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Sweep. 6 In the Sweep Feature dialog box, choose OK to accept the settings. Your drawing should look like this. Save your file.
Editing Sweep Features As with all sketched features, sweep features can be edited by modifying the profile, the path, or the feature itself. Try modifying the sweep features you just created. Creating Bend Features The bend feature is for bending flat or cylindrical parts. To create a bend feature, you sketch a single line segment on your part and create an open profile to define the tangency location where the part transitions from its current shape to the final bent shape.
To create a bend feature on a flat part 1 Use LINE to sketch a line on one side of the plate, responding to the prompts. Context Menu In the graphics area, right click and choose 2D Sketching ➤ Line. Specify first point: Select the start point of the line Specify next point [or Undo]: Select the end point of the line, and press ENTER 2 Use AMPROFILE to create an open profile, responding to the prompt. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile.
Choose OK. Hide the hidden lines to see your part better. To display silhouette edges, you set the DISPSILH system variable to 1 first. 5 Change the setting for DISPSILH. Command DISPSILH New value for DISPSILH <0>: Enter 1 6 Use HIDE to hide the hidden lines. Desktop Menu View ➤ Hide Your part should look like this. The bend is completed, and an icon for the bend feature is displayed in the Browser. Save your file.
166
Creating Work Features 9 In This Chapter In Autodesk® Mechanical Desktop®, work features are special construction features that you use to place ■ Work planes ■ Work axes ■ Work points geometry that would otherwise be very difficult to position parametrically. By constraining sketched and placed features to a work feature, that is in turn constrained to your part, you can easily control their location by changing the position of the work feature.
Key Terms Term Definition nonparametric work plane A work plane fixed in location with respect to a part. If the part geometry is parametrically changed, the work plane is unaffected. parametrics A solution method that uses the values of part parameters to determine the geometric configuration of the part. parametric work plane A work plane associated with and dependent on the edges, faces, planes, vertices, and axes of a part.
Basic Concepts of Work Features When you build a parametric part, you define how the part’s features are associated. Changing one feature directly affects all the features related to it. Work features are special construction features that help you define the relationships between the features on your part. They provide control when placing sketches and features. Any changes to the position of a work feature directly affect the placement of the sketches and features constrained to it.
Creating Work Planes A work plane is an infinite plane that you attach to your part. It can be either parametric or nonparametric. A work plane can also be used to define a sketch plane for new geometry. To position a feature that does not lie on the same plane as your base feature, you define a new plane and then create the feature. If the plane is parametric, any changes to it affect the position of the feature. Work planes are defined using two modifiers.
First, you create a work plane through the midplane of the part and extrude the profile to it. Later, you edit the position of the work plane to modify the depth of the new extrusion. Activate PART1_1 and use ZOOM to position it on your screen. Browser Double-click PART1_1. Now right-click PART1_1 and choose Zoom to. To create a work plane 1 Use AMWORKPLN to create a work plane through the midplane of PART1_1.
To extrude a profile to a plane 1 Use AMEXTRUDE to extrude the profile. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. 2 In the Extrusion dialog box, specify the following: Operation: Cut Termination: Plane Choose OK to exit the dialog box. 3 Continue on the command line. Select face or work plane: Specify the work plane The profile is extruded to the work plane. Now edit the location of the work plane to control the depth of the extrusion you just created.
Editing Work Planes Because a nonparametric work plane is static, any features constrained to it are restricted to the original plane. If you change the position or orientation of your part, the features remain associated with the work plane and your part could fail to update. Whenever possible, locate your features on parametric work planes. When you change the location of a parametric work plane, you change the position of any features created on it or constrained to it.
Creating Work Axes A work axis is a parametric construction line used as the axis of revolution for a revolved or swept feature, or an array of features; it is also used to place a work plane, and to locate new sketch geometry. You can create a work axis through the center of a cylindrical edge, or draw it on the current sketch plane by specifying any two points. PART2 contains a simple revolved feature, a work plane, and a partially constrained profile.
work axis Next, constrain the profile to the new work axis and create a revolved feature from it. Depending on your drawing, your default dimension values may differ from those in this exercise. To constrain and revolve a profile 1 Use AMPARDIM to constrain the profile to the work axis. Add two dimensions, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
2 Use AMREVOLVE to revolve a feature from the profile, responding to the prompt. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Revolve. Select revolution axis: Select the work axis 3 In the Revolution dialog box, specify: Operation: Cut Angle: Enter 360 Termination: By Angle Choose OK to exit the dialog box. Your drawing should look like this. Save your file.
Editing Work Axes Work axes are parametric, so any changes to the parameters controlling a work axis affect the location of features constrained to it. In this exercise, the work axis was created through the center of a cylindrical object and cannot be repositioned. But by changing one of the dimensions that constrains the profile to the axis, the revolved feature changes. To modify the revolved feature, you change the horizontal dimension constraining the profile to the work axis.
4 Use AMPARDIM to create a new parametric dimension, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Specify the right edge of the profile Select second object or place dimension: Specify the work axis Specify dimension placement: Place the dimension Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.4347>: Verify that the dimension is horizontal, then enter .15 Solved fully constrained sketch.
Creating Work Points A work point is a parametric point for positioning features that cannot easily be located on a part. By constraining a feature to a work point and then constraining the work point to the part, you control the position of the feature.
To create and constrain a work point 1 Use AMWORKPT to create a work point, responding to the prompt. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Work Point. Specify the location of the workpoint: Specify a point near the center of the sketch NOTE You may prefer to turn OSNAP off before you create and constrain the work point. Click the OSNAP button at the bottom of your screen. 2 Use AMPARDIM to constrain the work point to the work axis, following the prompts.
To solve a sketch and constrain it to a work point 1 Use AMPROFILE to solve the sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Profile. Select objects for sketch: Specify the polygon sketch Select objects for sketch: Press ENTER Solved underconstrained sketch requiring 8 dimensions or constraints. NOTE Although the polygon is a single object, you cannot use Single Profile to solve it because it was not the last object created.
To extrude a feature through a part 1 Change to an isometric view. Desktop Menu View ➤ 3D Views ➤ Front Right Isometric 2 Use AMEXTRUDE to extrude the profile through the part. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Operation: Cut Termination: Through Choose OK. The dimensions controlling the work point are still visible because the work point has not been consumed by a feature. Save your file.
To edit a work point 1 Use AMMODDIM to modify the vertical sketch dimension controlling the work point, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Edit Dimension. Select dimension to change: Specify the vertical dimension New value for dimension <0.6000>: Enter 0 Solved fully constrained sketch. 2 Use AMUPDATE to update the part, responding to the prompt. Context Menu In the graphics area, right-click and choose Update Part.
184
Creating Placed Features In This Chapter This tutorial introduces you to placed features, and builds on what you learned in previous tutorials. A 10 ■ Holes ■ Face drafts ■ Fillets placed feature is a well-defined common shape, such as ■ Chamfers a hole or a fillet. To create a placed feature, you only ■ Shells need to supply its dimensions. Autodesk® Mechanical Desktop® creates the feature for you.
Key Terms Term Definition chamfer A beveled surface between two faces. combine feature A parametric feature resulting from the union, subtraction, or intersection of a base part with a toolbody part. draft angle An angle applied parallel to the path of extruded, revolved, or swept surfaces or parts. A draft angle is used to allow easy withdrawal from a mold or easy insertion into a mated part. face draft A part face that has a draft angle applied to it.
Basic Concepts of Placed Features Placed features are well defined features that you don’t need to sketch, such as fillets, holes, chamfers, face drafts, shells, surface cuts, patterns, combined features, and part splits. You specify values for their parameters and then you position them on your part. To modify placed features, you simply change the parameters controlling them. Open the file p_feat.dwg in the desktop\tutorial folder.
Creating Hole Features You can create drilled, counterbore, and countersink hole features. Each may be assigned tapped hole information. Holes can extend through the part, stop at a defined plane, or stop at a defined depth. You can change a hole from one type to another at any time. When you create a hole, you can use the Thread tab in the Hole dialog box to include threads. Threads can also be added to existing holes.
2 Use AMHOLE to create two drilled holes. Context Menu In the graphics area, right-click and choose Placed Features ➤ Hole. NOTE Hold your cursor over an icon to see a tooltip that identifies the icon. In the Hole dialog box, on the Hole tab, select the Drilled hole type icon, and specify: Termination: Through Placement: Concentric Diameter: Enter .25 Choose OK to exit the dialog box.
3 Define the locations for the holes, responding to the prompts. Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]: Specify a face (1) Select concentric edge: Specify an edge (1) Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]: Specify a face (2) Select concentric edge: Specify an edge (2) Select work plane or planar face [worldXy/worldYz/worldZx/Ucs]: Press ENTER 1 2 Your drawing should look like this. Next, add internal threads to the HOLE_1.
To create a thread feature 1 In the Browser, select the hole to add threads. Browser Select Hole1. 2 Define the thread for Hole1 Context Menu In the graphics area, right-click and choose Placed Features ➤ Thread Respond to the prompts: Select cylindrical/conical edge or face: Select the circular edge of Hole1 Enter an option [Next/Accept] : Press ENTER In the Threads dialog box, specify: Thread Type: Custom Full Thread: Select the check box Major Dia: 0.2009 Minor Dia: 0.1709 Choose OK.
Editing Hole Features You can change a hole feature from one type of hole to another by modifying the parameters defining the hole. To edit a hole feature 1 Use AMEDITFEAT to change the second hole to a counterbore hole, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit.
Editing Thread Features You can redefine the size of an existing thread. If you need to change the thread type, it is necessary to delete the existing thread and create a new one. To edit a thread feature 1 Use AMEDITFEAT to change and display the thread feature, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit.
Creating Face Drafts Face drafts are used to add a small angle to one or more faces of a part; then the part can be easily extracted from a mold after it is manufactured. Face drafts can be applied from a specified plane, an existing part face, or a part edge. You can also create a shadow draft from a circular face. If you are creating a face draft from a plane, the plane can be either an existing face, or a work plane offset from the part. First, activate F-DRAFT_1 and zoom in on the part.
2 Choose Draft Plane and continue on the command line. Select draft plane (planar face or work plane): Specify the bottom face Draft direction [Accept/Flip] : Enter f to flip the direction arrow up Draft direction [Accept/Flip] : Press ENTER 3 In the Face Draft dialog box, in Faces to Draft, press Add. 4 Continue on the command line.
2 Respond to the prompts as follows: Select draft plane (planar face or work plane): Specify the back face Enter an option [Next/Accept] : Enter n to cycle to the back face, or press ENTER Draft direction [Flip/Next] : Enter f to flip the arrow away from the part, or press ENTER 3 In the Face Draft dialog box, specify: Faces to Draft: Add 4 Continue on the command line.
To create a shadow draft 1 Create the shadow draft. Context Menu In the graphics area, right-click and choose Placed Features ➤ Face Draft. In the Face Draft dialog box, specify: Type: Shadow Angle: Enter 45 Choose Draft Plane.
Editing Face Drafts To modify a face draft, you change the parameters that control it. To edit a face draft 1 Use AMEDITFEAT to change FaceDraft2, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit.
Creating Fillet Features Fillet features can range from simple constant fillets to complex cubic fillets. Mechanical Desktop creates the following fillet types: ■ ■ ■ ■ Constant Fixed width Linear Cubic A constant fillet has one radius defining it. A fixed width fillet is controlled by a chord length. Linear and cubic fillets have a radius at each vertex of the selected edges that you are filleting. A linear fillet has a straight transition from one vertex to the next.
2 Continue on the command line. Select edges or faces to fillet: Specify an edge (1) Select edges or faces to fillet: Specify an edge (2), and press ENTER 2 1 The fillets are applied to your part. Next, create a fixed width fillet where the cylindrical extrusion meets the angled face. To create a fixed width fillet 1 Use AMFILLET to create a fixed width fillet. Context Menu In the graphics area, right-click and choose Placed Features ➤ Fillet.
Your part should look like this. Create a linear fillet along the top left edge. To create a linear fillet 1 Create a linear fillet. Context Menu In the graphics area, right-click and choose Placed Features ➤ Fillet. In the Fillet dialog box, choose Linear, then choose OK. 2 Continue on the command line. Select edge: Specify the top left edge Select radius: Specify the back radius symbol Enter radius <0.5000>: Enter .35 and press ENTER Select radius: Specify the front radius symbol Enter radius <0.
To create a cubic fillet 1 Create a cubic fillet. Context Menu In the graphics area, right-click and choose Placed Features ➤ Fillet. In the Fillet dialog box, choose Cubic, then choose OK. 2 Continue on the command line. Select edge: Specify the top right edge at the back of the part Select radius or [Add vertex/Clear/Delete vertex]: Specify the back radius symbol Enter radius <0.5000>: Enter .
To edit a fillet 1 Use AMEDITFEAT to modify the cubic fillet, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit. Enter an option [Sketch/surfCut/Toolbody/select Feature]
Creating Chamfer Features A chamfer feature is a bevelled face created between two existing faces on a part. Chamfers can be created with an equal distance, two different distances, or a distance and an angle. You can select an edge or a face to place a chamfer. If one or more of the edges of a face you want to chamfer have been altered, you need to use the edge selection method to place chamfers around that face. First, activate CHAMFER_1 and zoom in on the part. Turn off the visibility of FILLET_1.
2 Choose OK and respond to the prompts as follows: Select edges or faces to chamfer: Specify an edge (1) Select edges or faces to chamfer : Press ENTER 1 Mechanical Desktop creates the chamfer along the edge you selected. You can also create chamfers by specifying two different distances. After you select the edge, you specify a face for Distance 1, called the base distance. Distance 2 is applied to the other face.
To create a chamfer defined by two distances 1 Use AMCHAMFER to create the chamfer. Context Menu In the graphics area, right-click and choose Placed Features ➤ Chamfer. In the Chamfer dialog box, specify: Operation: Two Distances Distance1: Enter .25 Distance2: Enter .15 Choose OK. 2 Respond to the prompts as follows: Select an edge or face to chamfer: Specify the edge (2) Press to continue: Press ENTER The specified face will be used for base distance.
To create a chamfer defined by a distance and angle 1 Define the chamfer. Context Menu In the graphics area, right-click and choose Placed Features ➤ Chamfer. In the Chamfer dialog box, specify: Operation: Distance and Angle Distance1: Enter 1 Angle: Enter 10 Choose OK. 2 Continue on the command line. Select an edge or face to chamfer: Specify the edge (3) Press to continue: Press ENTER The specified face will be used for base distance.
To create a chamfer on all edges of a face 1 Define the chamfer. Context Menu In the graphics area, right-click and choose Placed Features ➤ Chamfer. In the Chamfer dialog box, specify: Operation: Equal Distance Distance1: Enter .04 Choose OK. 2 Continue on the command line. Select edges or faces to chamfer: Select the face (4) Enter an option [Next/Accept] : Press ENTER Select edges or faces to chamfer : Press ENTER 4 A chamfer is placed on all edges of the face you selected.
Creating Shell Features You use shell features to hollow parts that are used in a variety of industrial applications. For example, you shell parts to create molds, castings, containers, bottles, and cans. Activate SHELL_1 and zoom in on it. Turn off the visibility of CHAMFER_1. The part is constructed from two extrusions and one fillet feature. Next, you shell the part, and then modify it to exclude the top and bottom faces. To create a shell feature 1 Use AMSHELL to create a shell.
Mechanical Desktop offsets all faces by the thickness you specified in the Shell Feature dialog box. 2 Change to a front view for a better view of the feature. Desktop Menu View ➤ 3D Views ➤ Front Save your file. Next, you edit the feature to exclude the top and bottom faces from the shell. Editing Shell Features You modify shell features by changing the parameters that control them. Shells can also have multiple thickness overrides applied to individual faces.
4 Continue on the command line. Select faces to exclude: Specify the bottom face Enter an option [Accept/Next] : Enter n to cycle to the bottom face Enter an option [Accept/Next] : Press ENTER Select faces to exclude: Specify the top face Enter an option [Accept/Next] : Enter n to cycle to the top face Enter an option [Accept/Next] : Press ENTER Select faces to exclude: Press ENTER Choose OK to exit the Shell Feature dialog box.
Creating Surface Cut Features Surface cut features give you the flexibility of combining a parametric part and a surface. While the surface is not parametric, its position on the part is controlled by a work point which you can move parametrically. Surface cut features may be used to add and remove material from a part. Activate SURFCUT_1 and zoom in to it. Turn off the visibility of SHELL_1. SURFCUT contains a simple rectangular extrusion, a work point, and a surface.
The Browser contains a surface cut icon at the bottom of the feature hierarchy for SURFCUT_1. Save your file. Next, you edit the position of the surface to modify the surface cut feature. Editing Surface Cut Features You can modify surface cut features in one of two ways: ■ ■ Parametrically change its position. Manually change the shape of the surface. In this section, you change the position of the feature by modifying the parametric dimensions controlling the work point associated with the surface.
2 Use AMMODDIM to change the vertical dimension controlling the work point, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Edit Dimension. Select dimension to change: Specify .75 New value for dimension <.75>: Enter .5 Select dimension to change: Press ENTER 3 Use AMUPDATE to update the part, responding to the prompt. Context Menu In the graphics area, right-click and choose Update Part.
While selecting a feature set for a pattern, you select each graphically dependent feature individually. You can select multiple independent features. Single instances in a pattern can be made independent of an existing pattern feature. Once a feature is independent, it can be altered while its position remains intact. In this tutorial, you create several different types of patterns, using both incremental and included spacing. In the polar pattern exercise, you make one instance independent and alter it.
2 In the Pattern dialog box, specify: Type: Rectangular Column Placement: Choose Incremental Spacing, the leftmost button Row Placement: Choose Incremental Spacing, the leftmost button NOTE Hold the cursor over an icon for a tooltip to identify the icon. Enter the values shown for column and row instances and spacing. 3 Choose Preview, and view your pattern on the screen. At this point, you can redefine the pattern by changing your selections in the Pattern dialog box, and then preview the changes.
Use R-PATTERN again to create a nonorthogonal rectangular pattern with included spacing and a value entered for the angle. In the Browser, right-click the icon for the pattern you just created, and choose delete. Verify that the R-PATTERN part is activated. To create a nonorthogonal rectangular pattern 1 Use AMPATTERN to create a nonorthogonal rectangular pattern, responding to the prompts. Context Menu In the graphics area, right-click and choose Placed Features ➤ Rectangular Pattern.
Next, create a full circle polar pattern using a work axis as the center and a specified number of instances. When you choose a different pattern type, the appropriate options are displayed in the Pattern dialog box. Activate P-PATTERN_1 and zoom to the part. The part is constructed with a circular plate and two holes. To create a polar pattern 1 Use AMPATTERN create a polar pattern, responding to the prompts. Context Menu In the graphics area, right-click and choose Placed Features ➤ Polar Pattern.
Choose Preview and view the pattern. Then choose OK. Next, make one instance of the pattern independent and then alter it. To make a pattern instance independent 1 Select the pattern instance to make independent. Browser Right-click PolarPattern, and choose Independent Instance. Respond to the prompts. Select feature pattern or array instance: Select hole instance #4 An independent hole based on a work point is copied from the selected hole instance.
The previous hole instance is suppressed. It can be reclaimed using the Pattern dialog box. 2 Use AMEDITFEAT to resize the independent pattern instance. Browser Right-click the independent Hole4, and choose Edit. The Hole dialog box is displayed. 3 In the Hole dialog box, change the diameter to .4, and choose OK. 4 Use AMUPDATE to update the part, responding to the prompt. Context Menu In the graphics area, right-click and choose Update Part.
To create an axial pattern 1 In the Browser, under A-PATTERN_1, right-click WorkAxis1 and choose Visible. 2 Use AMPATTERN to create an axial pattern, responding to the prompts. Browser In the Browser, right-click Polar Pattern1 and choose Pattern ➤ Axial.
5 Use HIDE to hide the hidden lines. Desktop Menu View ➤ Hide Your part should look like this. 6 Finish the part by using the new axial pattern to create another polar pattern. Browser In the Browser, right-click Axial Pattern1 and choose Pattern ➤ Polar. Select Rotational Center: Select the work axis 7 In the Pattern dialog box, specify: Polar Placement: Select Incremental Angle Instances: Enter 2 Spacing Angle: Enter 180 Choose OK. 8 Use HIDE to hide the hidden lines.
Editing Pattern Features You edit pattern features in the Pattern dialog box. In the Pattern Control tab, you modify the instancing controls. In the Features tab, you redefine the features in the pattern. Once a pattern is created, you cannot change the pattern type. When you delete a feature from a pattern set, you also remove other graphically dependent features that are children of that feature, such as fillets. If you want to add a feature to the set, a feature rollback is required.
Creating Copied Features You can copy a feature from any part, and place it on your active part on the current sketch plane. If the feature you select is on the active part, you can specify that the copy is independent. That way, you can modify either feature without affecting the other. If you do not specify that the copy is independent, or you copy a feature from an inactive part, any changes made to either the feature or the copy are reflected in both features.
To copy a feature 1 Use AMCOPYFEAT to create a copy of the slot, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Copy.
To constrain a copied feature 1 Use the Browser to edit the sketch. Browser Right-click ExtrusionBlind3 and choose Edit Sketch. 2 Use AMPARDIM to add three parametric dimensions to constrain the sketch to the part. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. 3 Place a 0.25 horizontal dimension, a 0.35 vertical dimension, and a 0.25 vertical dimension as illustrated below. 4 Use AMUPDATE to update your part, responding to the prompt.
Editing Copied Features You can edit a copied feature by modifying the feature itself, or by modifying its location on the part. If the copy is dependent on the original feature, or if it was created from a feature on an inactive part, any changes to either feature are reflected in both features. The copied feature you created is independent from the original feature. Try modifying the shape of the copied feature, using what you learned earlier in this tutorial about editing extrusions.
To create a combined feature 1 Use AMCOMBINE to create a combined feature, responding to the prompts. Context Menu In the graphics area, right-click and choose Placed Features ➤ Combine. Enter a parametric Boolean operation [Cut/Intersect/Join] : Select a part (toolbody) to be joined: Specify TOOLBODY_1 Enter j The parts are combined into one part. 2 Look at the Browser. Expand the Combine1 icon nested under COMBINEFEAT_1.
Creating Part Splits You can split parts by creating a planar or a nonplanar split feature. A planar split uses a work plane, existing part face, or a split line. A nonplanar split uses a constrained sketch and a Boolean operation. Activate P-SPLIT_1 and zoom in on the part. Turn off the visibility of COMBINEFEAT_1. The part is a simple extrusion with two holes and a work plane located at the midplane of the part. You split the part into two distinct part definitions with the work plane.
2 Expand PART2_1 in the Browser and compare its features with P-SPLIT_1. Both parts contain a Part Split feature, two holes, and a work plane. Save your file. You can also create planar splits with an existing part face, or a split line constrained to the part. Next, create a nonplanar split. Activate N-SPLIT_1 and zoom in on the part. Turn off the visibility of P-SPLIT_1 and PART2_1. NOTE For clarity, the profile’s dimensions are not shown.
2 Continue on the command line. Enter name of the new part : Press ENTER The part is split and a new part definition is created. Save your file. Editing Part Splits Parts created by a part split can be edited in the same way as the parts they were created from. The new parts contain identical work geometry, and if any feature was split, each part contains a version of that feature. Nonplanar splits are used to create parts that fit together.
232
Using Design Variables In This Chapter You can assign variables to the parametric dimensions 11 ■ Creating active part design variables that control a part. Variables can be assigned to the active part, or they can be global. ■ Assigning variables to an active part ■ Modifying design variables Active part design variables control only the features of ■ Creating global design variables the part they are assigned to. Global design variables control the features of any number of parts.
Key Terms Term Definition active part variable A parametric variable used in the dimensions that control features of the active part. global variable A parametric variable that can be used by any number of parametric features and parts. Also used for single parts and to constrain parts. helical sweep A geometric feature defined by the volume from moving a profile along a 3D path about a work axis.
Basic Concepts of Design Variables Parts and features are controlled by dimensions and other parameters that define their shapes. By creating design variables and assigning them to these parameters, you gain greater control over these values. There are two types of design variables: ■ ■ Global Active part You use global design variables when you want to control parameters that belong to more than one part. When you want to control only a specific part, you use active part design variables.
Three work planes are associated with the part. Two were used to create the sketched work axis for the sweep. The third, also called a profile plane, was created normal to the start of the path when it was defined. It was used to sketch the profile for the sweep. The profile is constrained to a work point at the beginning of the path. Preparing The Drawing File Before you begin, turn off the visibility of the work features.
To speed up recalculations and regenerations of the helical sweep, set the ISOLINES variable to its default value. This will display the sweep using only one wire. Currently it is set to display the sweep as a helical tube. To set isolines 1 Change the setting for ISOLINES, responding to the prompt. Command ISOLINES New value for ISOLINES <8>: Enter 4 2 Use REGEN to regenerate your drawing. Desktop Menu View ➤ Regen The helix should look like this.
To dynamically rotate a part 1 Use 3DORBIT to rotate the view of your part. Context Menu In the graphics area, right-click and choose 3D Orbit. 2 Select a point near the center of the part. This point acts as the central point for the rotation. Press the mouse button as you move your cursor around the screen. The part dynamically rotates as the cursor moves. 3 Release the mouse button when the display is to your liking. In the next procedure, you restore the view to its original display. The helix1.
Using Design Variables Design variables provide a tool for controlling dimensions, and using equations and relationships between dimensions. Changing one or more variables affects the entire part. Design variables can be either active or global. Active Part Design Variables Active part design variables control only the part they are assigned to. Global Design Variables Global design variables allow you to use the same variables for multiple features across multiple parts.
In addition to the method used in the following exercises, you can create design variables in the Equation Assistant dialog box while you are in the modeling process. In the Equation Assistant dialog box, you right-click in the variables list area and choose New. A space for the new variable is provided at the end of the list, and your cursor is positioned in the Name column. There you enter a name for the new variable, and then you define it in the Equation column.
4 Repeat step 3 to enter the following variables: Ht 2 Dia .5 Rad .05 Choose OK. The next step is to edit the existing part by replacing its dimensions with the design variables you have just created.
Assigning Design Variables to Active Parts Before the spring can be table driven, you need to assign the design variables you have defined. You edit the sweep feature and the profile used to create the sweep. You change the values controlling the feature with the design variables you have just created. To edit a sweep feature 1 Use AMDIMDSP to set dimensions to display as equations. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions as Equations.
4 Assign the last variable to the radius of the profile, responding to the prompts as follows: Select object: Select the dimension (1) Enter dimension value <.1>: Enter rad Select object: Press ENTER 1 NOTE For clarity, shading has been turned off in these illustrations. You may prefer to keep it on throughout the tutorial. 5 Use AMUPDATE to update the part, responding to the prompt. Context Menu In the graphics area, right-click and choose Update Part. The spring is updated.
Modifying Design Variables Design variables can be added and modified anytime during the design process. When the part is updated, changes to the design variables are automatically applied. In this exercise, you add a design variable for a taper angle on the active part. To add a design variable to an active part 1 Use AMVARS to add a design variable. Desktop Menu Part ➤ Design Variables 2 In the Design Variables dialog box, with the Active Part tab selected, choose New.
To modify a design variable 1 Use AMVARS to modify the design variable. Desktop Menu Part ➤ Design Variables 2 In the Design Variables dialog box, with the Active Part tab selected, highlight the taper variable. In the highlighted line, double-click the Equation field and enter 15. Choose OK to exit the Design Variables dialog box. 3 Use AMUPDATE to update the part. Context Menu In the graphics area, right-click and choose Update Part. Save your file.
Working with Global Design Variables You can assign global variables to more than one part to control similar features. In this lesson, you move some of the active part design variables to global variables and assign them to two parts. Open the file helix2.dwg in the desktop\tutorial folder. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40. The drawing contains two springs created from helical sweeps.
Next, examine the active part design variables for both parts. To examine a design variable for an active part 1 Use AMVARS to open the Design Variables dialog box. Desktop Menu Part ➤ Design Variables 2 In the Design Variables dialog box, with the Active Part tab selected, examine the values for the design variables assigned to PART1_1. You should see four variables controlling the number of revolutions, height, radius of the swept profile, and the taper angle of the active part.
5 In the Design Variables dialog box, make sure the Active Part tab is selected. Choose OK. Both parts have active part design variables controlling the same features. The variable controlling the height of both helical sweeps contains the same value. Next, you move this active part design variable to a global design variable so that one variable controls both parts. To move an active part variable to a global design variable 1 Open the Design Variables dialog box.
Choose OK to exit the dialog box. Mechanical Desktop re-evaluates the features of the part and updates the part. Because the value of the variable has not changed, the part does not change. Although the ht variable for PART2_1 has been moved to global, the same variable for PART1_1 is still an active part design variable. Because one global variable will drive both parts, you remove the ht variable from the PART1_1 list of active part design variables.
Next, you create a new global design variable to control the diameter of the springs and assign it to both parts. Then you modify the value of the global design variable controlling their height. To create a global design variable 1 Open the Design Variables dialog box. Desktop Menu Part ➤ Design Variables 2 In the Design Variables dialog box, select the Global tab and choose New. 3 In the New Part Variable dialog box, specify: Name: Enter dia Equation: Enter .75 Choose OK.
4 Continue on the command line. Select object: Press ENTER 5 Update the part. Context Menu In the graphics area, right-click and choose Update Part. Enter an option [active Part/Assembly/aLl parts/linKs] : Press ENTER Mechanical Desktop updates PART1_1 using the new global design variable to control the diameter of the sweep. PART1_1 6 Activate PART2_1. 7 Repeat steps 1 through 5 for PART2_1. Your drawing should look like this.
To modify a global design variable 1 Open the Design Variables dialog box. Desktop Menu Part ➤ Design Variables 2 In the Design Variables dialog box, with the Global tab selected, highlight the ht variable. In the highlighted line, double-click the Equation field and enter 1.25. Choose OK to exit the dialog box. Mechanical Desktop re-evaluates the features and updates both parts. Design variables are a powerful way to control the features of a part.
Creating Parts In This Chapter This tutorial continues with techniques you learned in 12 ■ Analyzing design ideas to simplify sketching previous lessons. You use sketches to create features. You position standard features, such as holes, and then ■ Selecting the base feature ■ Planning the order in which to add features combine them to create a part.
Key Terms Term Definition base feature The first feature you create. As the basic element of your part, it represents its simplest shape. All geometry you create for a part depends on the base feature. consumed sketch A sketch used in a feature, for example, an extruded profile sketch. The sketch is consumed when the feature is created. Desktop Browser A graphical representation of the features that make up your model.
Basic Concepts of Creating Parts You construct a model bit by bit, fashioning shapes to add to it and using tools to cut away the portions of the shapes you do not need. In Mechanical Desktop®, these shapes are the features of the part you are creating. Analyzing Rough Sketches You may be accustomed to jotting down design ideas on paper, starting with a rough outline for a part and adding details as you go.
The part is symmetrical. Visualize two perpendicular centerlines—one along the axis of the boss and another intersecting both lugs. As you create this part, consider this symmetry as you constrain features. As you build the saddle bracket, you learn to create features according to the relationships among them. In this case, the base feature of the part is the saddle and lugs. Because the remaining features attach to the saddle and lugs, you create the main shape first.
If you want to assign design variables as you are defining part sketches and creating features, use the Equation Assistant. You can activate the Equation Assistant in two ways: ■ ■ When you are prompted for a dimension value, right-click the graphics area. While you are creating sketched and placed features, in the feature dialog box, right-click a value field. For more information about working with design variables, see “Using Design Variables” on page 239. To begin this lesson, open the file saddle.
When you create these features, you position them symmetrically using a work axis and a work plane. Like other features, you include work features in your constraint scheme to maintain symmetry throughout future updates to the part. work plane work axis Sketching Base Features After you have a strategy, you are ready to sketch, constrain, and extrude the base feature of the part. Begin by creating a sketch of the block and then converting it to a profile sketch.
2 Use AMPROFILE to profile your sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. Mechanical Desktop analyzes the sketch and displays a message on the command line: Solved underconstrained sketch requiring 5 dimensions or constraints. NOTE Throughout this tutorial, the number of constraints your sketch needs may differ from the example, depending on how precisely you draw the sketch. You learn how to modify constraints so that your sketch solves correctly.
For this exercise, add dimensions in the order shown, starting with the dimension for the bottom line. Depending on your sketch, your default dimension values may differ from those in this exercise. To constrain a sketch 1 Use AMPARDIM to add parametric dimensions to fully constrain the sketch, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
3 5 4 2 1 3 Create the dimension for the top left horizontal line. Continue to follow the selection points. Select first object: Specify the left horizontal line (4) Select second object or place dimension: Place the dimension (5) Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.3951>: Enter .28 Solved underconstrained sketch requiring 2 dimensions or constraints. NOTE You may get a message stating that adding a dimension will overconstrain the sketch.
To extrude a feature 1 Change to an isometric view of your part. Desktop Menu View ➤ 3D Views ➤ Front Right Isometric You need to specify the type of extrusion operation, how to terminate the extrusion, and its size. 2 Use AMEXTRUDE to extrude the profile. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. 3 In the Extrusion dialog box, specify: Distance: .66 Termination: Blind Choose OK to create the feature. The base feature should look like this.
To edit a consumed sketch in the Browser, double-click the profile icon to display the original sketch, or right-click to show the menu, and choose Edit Sketch. Make any changes and choose Part ➤ Update to resize the part with the changed values. To edit a base feature 1 Select the sketch to edit, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit.
Creating Work Features Now that you have created the base feature, add the feature that defines the rough shape of the bracket. First, create work features to maintain symmetry. Then, use them to draw, constrain, and extrude the sketch. The first work feature is a work axis along the centerline of the arc on the base feature. This work axis anchors your next sketch to the base feature. To create a work axis 1 Use AMWORKAXIS to create the work axis, responding to the prompt.
work plane To locate the work plane parametrically, specify the offset depth as an equation. By using an equation, the work plane tracks changes in the bracket width and always remains centered. To use an equation, you must determine the dimension parameter before you define the work plane. To create a work plane 1 Use AMDIMDSP to set dimensions as equations. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions as Equations.
4 Press ENTER to exit the command. 5 Create a parametric work plane in the center of the part, parallel to the front surface, and offset one-half the width of the part. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Work Plane.
The work plane is displayed as a planar rectangle. The Desktop Browser displays both a work axis and a work plane icon. work plane work axis Save your file. Defining Sketch Planes Before you can sketch the next feature, you must define a new sketch plane, an infinite XY plane that locates a 2D sketching surface in 3D space. When you create sketched features, you determine the placement and orientation of the sketch plane on a 2D plane.
As you move your mouse over a part, Mechanical Desktop highlights the faces that can be used to define a new sketch plane. Faces that cannot be used are not highlighted. When you select a face, a temporary sketch plane appears on that face. temporary sketch plane You can choose the Z direction and orientation of the XY axes for the new sketch plane. After you have selected the options, the temporary sketch plane disappears from the screen. You are ready to create the sketch geometry.
3 Use AMSKPLN to create a new sketch plane for the profile to be extruded, responding to the prompts. Context Menu In the graphics area, right-click and choose New Sketch Plane.
Creating Extruded Features To define the rough shape of the saddle bracket, you sketch a diamond shape with filleted corners and add constraints to stabilize its shape. When the feature is stabilized with geometric constraints, you add dimensions to fully define its size. Finally, you extrude the sketch, creating a solid feature from the combined volume of the original base feature and the extruded feature. To create a profile sketch 1 Use PLINE to sketch this shape in the left viewport.
2 Use AMPROFILE to create a profile from the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. Mechanical Desktop analyzes the sketch, redraws it, and displays this message: Solved underconstrained sketch requiring 10 dimensions or constraints. NOTE If your sketch needs more than 10 dimensions or constraints to solve the sketch, you probably need some tangency and constraints. Look for sharp discontinuities between the fillets and the lines they join.
To geometrically constrain a sketch 1 Use AMADDCON to add tangent constraints to the arcs and lines, following the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Tangent.
2 Select the arcs to constrain, following the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Radius. Valid selection(s): arc or circle Select object to be resized: Select the arc at the top of the sketch (1) Valid selection(s): arc or circle Select object radius is based on: Select the arc at the bottom of the sketch (2) Solved underconstrained sketch requiring 9 dimensions or constraints.
4 Delete any parallel constraints, responding to the prompts If your sketch doesn’t contain parallel constraints, skip this procedure. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Delete Constraints. Select or [Size/All]: Specify the constraint with the P symbol (1) Select or [Size/All]: Specify the constraint with the P symbol (2) Select or [Size/All]: Press ENTER 1 2 These parallel constraints, although valid, conflict with adding dimensions between arc centers.
To dimension a sketch 1 Use AMDIMDSP to change the dimension display back to numbers. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions as Numbers. 2 Use AMPARDIM to dimension the radius for the top and right arcs, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
4 Create a horizontal dimension between the centers of the left and right arcs. Select first object: Specify the left arc center (1) Select second object or place dimension: Specify the right arc center (2) Specify dimension placement: Place the dimension (3) Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.9797>: Press ENTER 5 4 1 2 3 5 Dimension the distance between the centers of the top and left arcs.
rough shape rough shape as a part To constrain a sketch to a base feature 1 Use AMADDCON to make the center of the right arc lie on the work plane, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Project.
2 Make the center of the left arc lie on the work plane. Valid selection(s): line, circle, arc, ellipse or spline segment Specify a point to project: Enter cen of: Specify the arc (1) Valid selection(s): line, circle, arc, ellipse, work point or spline segment Select object to be projected to: Specify the work plane (2) 1 2 3 Position the center of the top arc on the work plane.
4 Position the center of the top arc on the work axis. Valid selection(s): line, circle, arc, ellipse or spline segment Specify a point to project: Enter cen of: Specify the arc (1) Valid selection(s): line, circle, arc, ellipse, work point or spline segment Select object to be projected to: Specify the work axis (2) 1 2 5 Use AMADDCON to make the center of the bottom arc concentric with the center of the top arc, responding to the prompts.
Your sketch should be fully solved and look like this. Save your file. Editing Sketches Now that the sketch is fully constrained, you can change the sketch dimensions to position the sketch on your part. Modify the distances between the center of the left arc and the center of the sketch and between the centers of the left and right arcs. To change a sketch dimension 1 Use AMMODDIM to modify the values of the dimensions, following the prompts.
Your part should look like this. Now, you need to create an equation between the overall dimension and the dimension that centers the feature on the part and maintains symmetry relative to the work axis. Display the dimensions as parameters, and then use them as variables in the parametric equation. 2 Use AMDIMDSP to display the dimensions as parameters. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions As Parameters.
Now that the profile sketch is completely constrained and dimensioned, you can use it to change the shape of the base feature. Extruding Profiles You create a solid feature by extruding the profile through to the boundary of the base feature, retaining the common volume. To create the rough shape of the saddle bracket, you extrude the profile sketch up and completely through the base feature. Because the sketch you extrude changes the shape of the base feature, the intersection shares the volume of both.
To extrude a profile through a base feature 1 Use AMEXTRUDE to create the extrusion. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, accept the default size and specify: Operation: Intersect Flip: Verify that the direction arrow is pointed up through the part Termination: Through Choose OK to exit the dialog box and create the extrusion. Save your file.
Creating Revolved Features With the rough shape of the saddle bracket defined, you can create the next dependent feature, the boss, which is a cylinder. The fastest and most efficient method to model the cylindrical boss is to extrude a circle. Alternatively, you can revolve a rectangle about a central axis. This method is used here to teach you the revolving method. When you finish the exercise, your model will look like this.
2 A work axis passes vertically through the part. If the work axis is not displayed, use AMVISIBLE to display it. Desktop Menu Part ➤ Part Visibility In the Desktop Visibility dialog box, choose the Part tab and check Work Axes. Select Unhide and choose OK. Next, you need to create a new sketch plane. Because the cylinder is vertical, you place the sketch plane on the previously defined work plane. 3 Create a new sketch plane, responding to the prompts.
5 Make the left viewport active and change the view so that you see a front view of the part as you look at the sketch plane. Desktop Menu View ➤ 3D Views ➤ Front 6 Sketch a rectangular outline of the cylinder, following the prompts. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Rectangle.
To constrain a profile sketch to revolve 1 Use AMDIMDSP to change the dimension display to numbers. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions as Numbers. 2 Use AMPARDIM to dimension the length and width of the sketch, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
3 Use AMADDCON to add collinear constraints, following the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Collinear. Valid selections: line or spline segment Select object to be reoriented: Specify the line (1) Valid selections: line or spline segment Select object to be made collinear to: Specify the vertical work axis (2) Solved underconstrained sketch requiring 1 dimensions or constraints.
To revolve a feature about a work axis 1 Use AMREVOLVE to revolve the sketch about the work axis, responding to the prompt. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Revolve. Select revolution axis: Specify the axis (1) 1 2 In the Revolution dialog box, specify the operation, termination, and angle of revolution. Because the cylinder attaches to the part, define the revolution to be a full (360 degrees) termination that joins to the part.
After specifying the type of revolution and the axis of rotation, the cylinder is created on your model. Save your file. Creating Symmetrical Features The final features are the strengthening ribs, located on each side of the saddle just above the lugs. strengthening rib The ribs can be created simultaneously from a single open profile sketch. You sketch an outline of the ribs, and add dimensions and constraints to make the ribs symmetrical. Then you extrude the ribs automatically with the Rib feature.
To sketch a feature on a part 1 Use PLINE to sketch the ribs. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Polyline. Sketch a three-segment polyline in the approximate outline of the ribs. The lines don’t have to touch the saddle. 2 Use AMPROFILE to create an open profile from the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. Respond to the prompt.
To constrain a sketch 1 Use AMPARDIM to dimension the distance between the top of the sketch and the top of the part. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Respond to the prompts as follows: Select first object: Specify the line (1) Select second object or place dimension: Specify the line (2) Specify dimension placement: Place the vertical dimension (3) Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.1683>: Enter .
3 5 4 1 2 3 Add horizontal dimensions for the top line of the sketch, and from the work axis to the outer edge of the top line. Select first object: Specify the line (1) Select second object or place dimension: Place the horizontal dimension (2) Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.9806>: Enter .
To display the dimensions as parameters 1 Use AMDIMDSP to change the display of the dimensions from numeric to parametric. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions As Parameters. Display the dimensions as equations. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Dimensions As Equations. 2 Use AMMODDIM to edit the dimensions. Use the work axis as the centerline of the part.
3 Use AMUPDATE to apply any changes to the rib sketch. Context Menu Right-click the graphics area and choose Update Part. You are ready to extrude the sketch to form symmetrical ribs. 4 Use 3DOrbit to adjust the view so you can see the rib feature preview before you create the ribs. Desktop Menu Choose View ➤ 3D Orbit. Rotate the view slightly to the left, and tilt it slightly downward. 5 Use AMRIB to extrude the ribs. Browser In the Browser, right-click the open profile icon, and choose Rib.
To suppress silhouette edges from Mechanical Desktop parts 1 Set the DISPSILH system variable to 1, responding to the prompts. Command DISPSILH Enter new value for DISPSILH <0>: Enter 1 2 Use HIDE to remove the hidden lines from your display. Desktop Menu View ➤ Hide Your part should now look like this. The Desktop Browser shows the hierarchy of the part features. 3 Return to wireframe display. Desktop Menu View ➤ Shade ➤ 3D Wireframe Save your file.
Refining Parts Now, you complete the part by modifying its features in the same order as you created them: the saddle and lugs, the boss, and the ribs. To finish the body of the saddle bracket, you need to cut the pipe saddle, adjust the length of the lugs, and create mounting holes. To create the saddle, you cut an arc through the front of the saddle body. To cut the arc, you create a circle and extrude it through the part, along the horizontal work axis.
3 Use AMADDCON to constrain the circle to be concentric with the saddle arcs, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Concentric.
5 Use AMPARDIM to dimension the diameter of the circle, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Specify the circle (1) Select second object or place dimension: Place the dimension (2) Enter dimension value or [Undo/Placement point] <1.0976>: Enter 1.12 Select first object: Press ENTER 2 1 The sketch is now fully constrained and looks like this.
To extrude a feature 1 Extrude the feature, specifying a cut operation with a midplane termination. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. 2 In the Extrusion dialog box, specify: Operation: Cut Distance: Enter .66 Termination: Type: Mid Plane Choose OK. The arc shape cuts through the saddle bracket. To complete the body of the bracket, you need a placed feature on each of the lugs for mounting holes.
3 Respond to the prompts as follows: Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]: Specify face (1) Enter an option [Next/Accept]: Press ENTER Select the concentric edge: Specify edges (1) for the first hole 2 1 4 Continue on the command line to place the second hole.
To create a counterbored hole 1 Use AMHOLE to place the counterbored hole. Context Menu In the graphics area, right-click and choose Placed Features ➤ Hole. In the Hole dialog box, select the Counterbore hole type icon and specify: Termination: Through Placement: Concentric Hole Parameters: Size: Enter .42 C’Bore/Sunk Size: C’ Dia: Enter .48 C’Bore/Sunk Size: C’ Depth: Enter .125 Choose OK.
To edit a feature 1 Use AMEDITFEAT to edit the rib sketch. Browser Right-click OpenProfile1 and choose Edit Sketch. The rib sketch and its dimensions become visible on the screen. 2 Change two of the dimensions in the sketch, following the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ Edit Dimension. Select object: Specify the dimension (1) Enter new value for dimension <40>: Enter 28 Select object: Specify the dimension (2) Enter new value for dimension <.
Shading and Lighting Models To see your model better, use the shade button on the Desktop View toolbar to toggle shading on. Then adjust the lighting of your shaded model. To toggle shading of a part 1 Use SHADE to shade your part. Desktop Menu View ➤ Shade ➤ Gouraud Shaded Your part should now look like this. The Desktop View toolbar also contains commands to dynamically rotate your design and control views. Now adjust the ambient and direct lighting of your shaded part.
To control the lighting of a shaded part 1 Use AMLIGHT to adjust the intensity of ambient and direct light. Toolbutton Lighting Control In the Lights dialog box, use the slider bars to adjust the intensity of the ambient light and the direct light as follows. 2 Use AMLIGHTDIR to specify a direction for direct light. In the Lights dialog box, click the Light Direction button.
306
Creating Drawing Views In This Chapter Autodesk® Mechanical Desktop® simplifies both the 13 ■ Planning and setting up your drawing drawing and the documentation of your design. Drawing views are associated with a part and with one another. You lay out drawing views in any position on a ■ Multiple document layouts ■ Creating drawing views ■ Hiding extraneous dimensions ■ Moving dimensions to a different screen. You can move them and make changes easily.
Key Terms Term Definition balloon A circular annotation tag that ties components in an assembly into a bill of material. base view The first view you create. Other views are derived from this view. Desktop Browser A graphical representation of the features that make up your model. You can work in the Browser to create and restructure parts and assemblies, define scenes, create drawing views, and control overall preferences.
Basic Concepts of Creating Drawing Views Drawings and documentation are often the true products of design because they guide the manufacture of a mechanical device. Mechanical Desktop adds an important dimension to drawing creation by doing most of the work for you. Traditional 2D orthographic, isometric, auxiliary, section, and detail views of parts and assemblies can be automatically created. Mechanical Desktop creates these views complete with dimensions derived from the models.
Creating Drawing Views The first view you create is a base view. In Model mode, you specify the orientation of the view, and then change to Drawing mode to position it on the page. A title block and drawing border have been placed on the TITLE_BLK layer. When you place the base view, hidden lines are removed. Parametric dimensions are shown according to the currently-defined dimension style.
2 Respond to the prompts as follows: Select a planar face, work plane, or [Ucs/View/worldXy/worldYz/worldZx]: Specify the work plane (1) Define X axis direction: Select work axis, straight edge or [worldX/worldY/worldZ]: Specify the axis of revolution (2) Adjust orientation [Flip/Rotate] : Enter r until the UCS icon is upright, or press ENTER 1 2 3 On the command line, define a location on the drawing for the base view.
The base view is placed at the location you selected. The Desktop Browser displays a hierarchy of the views you create. Because you have only the base view, it is listed below the part. As you create views from the base view, they are nested beneath the base view in the Browser. Because the base view is too small to be easily read, enlarge it by changing the view scale. Subsequent views will use the enlarged view scale until you specify a different one. 4 Use AMEDITVIEW to edit the scale of the base view.
To create a top and detail view 1 Create the orthographic view. Context Menu In the graphics area, right-click and choose New View. In the Create Drawing View dialog box, specify the Ortho view type and Choose OK. 2 Define a location for the orthographic view, responding to the prompts.
Because the orthogonal view is created from the base view, it is nested below the Base icon in the Desktop Browser. Next, create an independent detail view of one of the lugs. Properties of independent detail views can be changed without affecting the properties of the parent view. To create a detail view, choose the parent view and the area in the parent to show in detail. In this case, create a detail view of the rightmost mounting lug. For detail views, you always define the viewport border.
2 Define the detail view, responding to the prompts.
Your drawing should look like this. The Browser displays a Detail icon nested below the Ortho icon. 3 Use AMEDITVIEW to edit the edge properties of the detail view. Context Menu In the graphics area, right-click and choose Edit View. Select the detail view you created. In the Edit Drawing View dialog box, select the Display tab, and select Edge properties. 4 Edit the detail view edge properties, responding to the prompts.
The lug color in the detail view changes to red. However, the lug color remains unchanged in the parent view. For practice, create the same detail view using a circle for selection. Notice how the command line prompts change according to the selection type you use. Next, you create a cross section—a view that cuts through a point on the part along a work plane, or if the part is an offset section, through a sketch. Work planes are often easier to visualize and select than cutting planes.
3 On the command line, respond to the prompts as follows. Select work axis, straight edge or [worldX/worldY/worldZ]: Specify the work axis (1) Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]: Specify the work plane (2) 2 1 Your model should now look like this. Next, you create a full cross-section view of the part that is an orthographic projection of the front view. 4 Return to Drawing mode. Browser 318 | Select the Drawing tab.
5 Create a new drawing view. Context Menu In the graphics area, right-click and choose New View. In the Create Drawing View dialog box, specify: View Type: Ortho Choose the Section tab and specify: Type: Full Label: Enter A Label Pattern: Section A-A Hatch: Select the check box, and press Pattern Use the Hatch Pattern dialog box to define the hatch pattern, and choose OK. Choose OK to close the Create Drawing View dialog box. 6 Define the orthogonal view, responding to the prompts.
Your display should now look like this. 7 Create an isometric view, using the base view as the parent view. Context Menu In the graphics area, right-click and choose New View. In the Create Drawing View dialog box, specify: View Type: Iso Scale: Enter 1 Relative to Parent: Select the check box Choose OK. 8 Define the isometric view, responding to the prompts.
2 1 Your drawing should look like this.
Each drawing view is represented as it relates to other views. For example, the ortho, section, and iso views are derived from the base view. Also, it is clear that the detail view is based on the ortho view. Detail and section views are named according to the labels you specified. Save your file. Cleaning Up Drawings After creating the drawing views, you need to clean up the parametric dimensions and some extraneous lines. Parametric dimensions are automatically placed on the AM_PARDIM layer.
To hide extraneous dimensions in a front view 1 Zoom to the base view. Context Menu In the graphics area, right-click and choose Zoom. 2 Activate the Desktop Visibility dialog box. Desktop Menu Drawing ➤ Drawing Visibility In the Desktop Visibility dialog box, verify that the Hide option is selected. Then choose Select. 3 On the command line, respond to the prompts to select the redundant .33 and .74 dimensions to hide. Select drawing objects to hide: Specify the 0.
4 Your display should look like this. In the top view, the 1.16 dimension specifies the distance between arc centers. You can hide the extraneous .58 and 0.08 dimensions. To hide extraneous dimensions in a top view 1 Zoom to the top view. Browser Right-click Ortho and choose Zoom to. 2 Activate the Desktop Visibility dialog box. Desktop Menu Drawing ➤ Drawing Visibility 3 In the Desktop Visibility dialog box, verify that the Hide check box is selected and choose Select.
Moving Dimensions Mechanical Desktop places dimensions on the drawing according to the way they were created during sketching. Usually, some cleanup is required, to comply with drafting standards. In the following exercises, you will move dimensions within and between views until all the dimensions needed to define the part are visible on the drawing. All the dimensions for the drawing currently exist in the front and top views. Originally these views were cluttered with extraneous dimensions.
3 Continue moving dimensions until the front view looks like this. 4 Zoom to the top view. Browser Right-click Ortho and choose Zoom to. 5 Use AMMOVEDIM to move some of the dimensions in the top view. Context Menu In the graphics area, right-click and choose Annotate Menu ➤ Edit Dimensions ➤ Move Dimension. Follow the command line prompts to move dimensions until your view looks like this.
To move a dimension to a different view 1 Zoom in to view the front and cross-section views. Context Menu In the graphics area, right-click and choose Zoom. 2 Use AMMOVEDIM to move a dimension from the front view to the crosssection view, following the prompts. Context Menu In the graphics area, right-click and choose Annotate Menu ➤ Edit Dimensions ➤ Move Dimension. Enter an option [Flip/Move/move mUltiple/Reattach] : Press ENTER Select dimension to move: Specify the 0.
Hiding Extraneous Lines Although Mechanical Desktop eliminates lines when it creates views, you may want to edit the views to remove additional, unwanted lines. To hide an extraneous line 1 Zoom to the isometric view. Browser Right-click Iso and choose Zoom to. 2 Use AMEDITVIEW to edit the Iso view. Context Menu In the graphics area, right-click and choose Drawing Menu ➤ Edit View. 3 Specify the isometric view.
5 On the command line, respond to the prompts as follows: Enter an option (edge properties) [Remove all/Select/Unhide all]
Enhancing Drawings When you are satisfied with the drawing views, you can modify and enhance them. Enhancements include: ■ ■ ■ ■ Adding more dimensions Adding annotations such as callouts, hole notes, and centerlines Relocating views Modifying the part from the drawing view Changing Dimension Attributes Even though you set up the dimension style before creating the dimensions, some dimensions may need to be displayed in a particular way.
4 Choose the General tab. The .12 dimension should now be expressed as 0.120 +/- .001. Now that the dimension is longer, it may overlap the drawing view. Choose OK. 5 Move the dimension so that it does not overlap any geometry. Context Menu In the graphics area, right-click and choose Edit Dimensions ➤ Move Dimension. Move the dimension so that it looks like this.
Creating Reference Dimensions You can supplement parametric dimensions with reference dimensions. The reference dimensions do not control the size of the model; however, if you change the model, the reference dimensions are updated to reflect the new size. Reference dimensions reside on the AM_REFDIM layer. In the next exercise, you add a reference dimension to the front view. To add a reference dimension 1 Zoom to the front view. Browser Right-click Base and choose Zoom to.
Creating Hole Notes Mechanical Desktop does not automatically display hole dimensions on the drawing, but you can add this information. First, you add a hole note to the boss in the top view, and tapped hole information to the mounting hole in the detail view. To create a hole note 1 Zoom to the top view. Browser Right-click Ortho and choose Zoom to. 2 Use AMNOTE to create a hole note for the hole through the boss, responding to the prompts.
3 In the Note Symbol dialog box, choose the more button to display the Note Templates section. In Note Templates, choose the COUNTER BORE template. 4 Select the Leader tab, and set the leader justification to Middle of All Text. Choose OK. A hole note with the hole diameter, the counterbore diameter, and the hole depth is displayed on your drawing. Next, add hole information to the mounting hole in the detail view.
To create a modified hole note 1 Zoom to the detail view. Browser Right-click Detail and choose Zoom to. 2 Create the hole note, responding to the prompts. Context Menu In the graphics area, right-click and choose Annotation ➤ Hole Note. Select object to attach [rEorganize]: Specify the hole in detail view (1) Next Point : Specify the location (2), and press ENTER. 1 2 3 In the Note Symbol dialog box, choose the more button to display the Note Templates section.
Creating Centerlines In this exercise, you create a parametric centerline for the top view and a center mark for the detail view. Centerlines and center marks are attached to the view and move with the view as the model changes. To create a centerline 1 Add a center mark, responding to the prompts. Context Menu In the graphics area, right-click and choose Annotation ➤ Centerline.
1 2 A centerline is placed through the view. Now, specify where to trim the centerline endpoints. Select first trim point: Specify a point to the right of the part Select second trim point: Specify a point to the left of the part Your display should look like this. Creating Other Annotation Items When you make changes to a model, the geometry and dimensions are updated automatically. Special commands create drawing annotations such as reference dimensions, hole notes, and centerlines.
To convert a callout bubble 1 Zoom out to view the entire drawing. Context Menu In the graphics area, right-click and choose Zoom. Rightclick again and choose Zoom Extents. Right-click again and choose Exit. 2 Use LAYER to turn on the AM_ANNOTE layer. You should see a callout bubble containing the number 1 and a leader. 3 Use AMMOVEVIEW to position the isometric view near the callout, responding to the prompts. Context Menu In the graphics area, right-click and choose Drawing Menu ➤ Move View.
4 Convert the callout bubble to an annotation, responding to the prompts. Context Menu In the graphics area, right-click and choose Annotation Menu ➤ Annotation ➤ Create Annotation. Select objects to associate with view: Draw a selection rectangle around the callout bubble, numeral, and leader (1, 2) Select objects: Press ENTER Select point in view to attach annotation: Specify a point (2) 1 2 Your drawing should look like this.
Modifying Drawing Views You can relocate views or change the model from a drawing view. The drawing and, if appropriate, the model, are updated to reflect the changes you made. Move the isometric view. The callout bubble moves with the view because it is associated with the part. Then, relocate the isometric and detail views, and change the detail view. The model and all drawing views are updated. To relocate a drawing view 1 Move the Iso view back to its former location, responding to the prompts.
2 Relocate the detail view to the right of and below the isometric view, responding to the prompts. Context Menu In the graphics area, right-click and choose Move View. Select view to move: Specify center of the detail view (1) Specify new view location: Specify new location (2) and press ENTER Specify new view location: Press ENTER 1 2 All annotations associated with the view move with it and keep their positions relative to the view. You can move views from layer to layer.
To modify a drawing view 1 Zoom to the top view. Context Menu In the graphics area, right-click and choose Zoom. 2 Use AMMODDIM to change the radius of the lug, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Dimensions ➤ Edit Dimension. Select dimension to change: Select the .16 value of the lug radius New value for dimension <.16>: Enter .13 Select dimension to change: Press ENTER You must update the part to show the changes.
Exporting Drawing Views You can save your 2D drawing views directly to Mechanical Desktop versions other than Release 6 as DWG, DWT, or DXF files. You can export the entire current layout, including all views and geometry, or you can select views and entities to export.
To export Mechanical Desktop drawing views 1 Use AMVIEWOUT to save your drawing view file to AutoCAD 2000. Browser In the Browser, right-click Base and choose Export View.
Creating Shells In This Chapter This tutorial teaches you how to create and edit a 14 ■ Adding a shell feature to an existing part shelled part in Autodesk® Mechanical Desktop®. With the shell feature, you can create complex parts with ■ Modifying wall thickness ■ Adding multiple thickness overrides walls of varying thickness. In the tutorial, you add a ■ Managing thickness overrides shell feature to an existing die cast engine part, and then edit the shell.
Key Terms Term Definition converging radial shapes A sharp corner where cylindrical faces, such as fillets, are offset and converge to form a zero radius. Parts with more complex shapes, such as variable radius fillets and surfcuts, need a shell thickness large enough so that the offset face does not converge. default thickness The offset value initially applied to all faces of your part. excluded face Face on a shelled part you select that will not be offset.
Basic Concepts of Creating Shells Unlike other sketched or placed features, a shell feature is initially applied to all the faces of your active part, instead of only those you select. It doesn’t need parametric dimensions to control placement. A part can have only one shell feature. When you add a shell feature to a part, Mechanical Desktop creates new faces by offsetting existing ones inside or outside of their original positions.
Using Replay to Examine Designs First, review the clutch housing design. Open the file clutch.dwg in the desktop\tutorial folder. The clutch housing has been modeled to a point in the design where it is ready for you to add the shell feature. It contains six extruded features. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
This displays the model in another isometric view. Next, you remove the silhouette edges from your model so you can visualize it better. Silhouette edges are similar to hidden lines, but to remove them you need to modify a system variable. 3 Change the system variable controlling the visibility of silhouette edges. Command DISPSILH New value for DISPSILH <0>: Enter 1 4 Use HIDE to remove hidden lines from your display. This improves your view of the features of the housing.
Cutting Models to Create Shells Now that you have examined the model, the next step is to cut it, removing the interior area, so that all that remains is a shell of the part. This part is a magnesium alloy casting which requires a wall thickness of about 4 mm in most areas, but some walls must be thicker to withstand forces applied to them. To cut a model 1 Return to the back right isometric view. Desktop Menu View ➤ 3D Views ➤ Back Right Isometric 2 Return to a wireframe display of your model.
The shell feature is calculated and the model is updated. 5 Change your display to three viewports. Command 3 This gives you a better view of the thickness of the walls in the model. An isometric view of the bottom of the housing has been previously saved. 6 Click in the right viewport to make it current, and restore the saved view. Desktop Menu View ➤ Named Views 7 In the View dialog box, highlight BOTTOM_ISOMETRIC and choose Set Current. Choose OK.
When the shell feature was added, all the faces in the model were offset. The result is a hollow model. For a better view, suppress the hidden lines. 8 Use HIDE to remove the hidden lines. Desktop Menu View ➤ Hide Save your file. Editing Shell Features When you create a shell, your wireframe display becomes more complex because Mechanical Desktop offsets each face in your model, doubling the number of faces. One way to edit a shell feature is to use AMEDITFEAT and select an offset face edge.
To exclude a face on a shell feature 1 Use AMEDITFEAT to edit the shell feature. Browser In the Browser, right-click Shell1 and choose Edit. If you choose a method other than the Browser, you must select the shell feature first. The Shell Feature dialog box is displayed.
3 Use AMUPDATE to update the part, responding to the prompt. Context Menu In the graphics area, right-click and choose Update Part. Enter an option [active Part/aLl parts] : Press ENTER The model is updated to reflect the modified shell feature. Save your file. Adding Multiple Wall Thicknesses When the clutch housing is attached to an operating engine, the stresses are higher on some casting walls than on others.
To edit a shell through the Browser 1 Return to the back right isometric view. Desktop Menu View ➤ 3D Views ➤ Back Right Isometric The face surrounding the water pump can now be selected easily. 2 Return to a wireframe display of your model. Desktop Menu View ➤ Shade ➤ 3D Wireframe 3 Edit the shell feature again. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit. Select the shell feature. The Shell Feature dialog box is displayed.
5 Update the part, responding to the prompt. Context Menu In the graphics area, right-click and choose Update Part. Enter an option [active Part/aLl parts] : Press ENTER Refer to the top view in the upper left viewport to see the results. When you selected the cylindrical face, tangent faces were automatically selected. The wall thickness surrounding the water pump should look twice as thick as the rest of the walls.
3 In the Shell Feature dialog box, specify: Multiple Thickness Overrides: New Thickness: Enter 6 Choose Add, and respond to the prompts as follows: Select faces to add: Specify a point on the model (1) Select faces to add: Specify a second point (2) Select faces to add: Press ENTER Choose OK to exit the dialog box. 1 2 4 Update the part. Context Menu In the graphics area, right-click and choose Update Part. In the top view, the two faces you selected are thicker.
6 In the View dialog box, highlight BOTTOM_PERSPECTIVE, choose Set Current, and then choose OK. 7 Use HIDE to remove the hidden lines. Desktop Menu View ➤ Hide Save your file. Managing Multiple Thickness Overrides Occasionally, you may create complex parts that require more thickness override values. As you apply the override values to faces on your part, it is easy to lose track of which faces are using different overrides, especially if you are viewing a part that was designed by someone else.
For the clutch assembly, the wall thickness around the water pump can be reduced from 6 to 4. Because the default wall thickness of the shell is 4, you remove the override of 6 from the list. When you delete an override value from the list, faces that once referenced that value revert to the default thickness. To change a wall thickness 1 Use AMEDITFEAT to edit the shell feature again to change the wall thickness around the water pump.
360
Creating Table Driven Parts In This Chapter You can assign variables to the parametric dimensions that control a generic part and then use a table (an 15 ■ Creating a table ■ Displaying part versions ■ Editing a table external spreadsheet) to control the size and shape of the part. The spreadsheet can contain several versions of ■ Solving common problems with table driven parts ■ Suppressing features in table the part. Each version uses different values for the variables you define.
Key Terms Term Definition active part variable A parametric variable used in the dimensions that control features of the active part. feature suppression Temporarily removing features from the calculation of a part. Features can be suppressed manually through the Desktop Browser, or through a linked external table. global variable A parametric variable that can be used by any number of parametric features and parts. Also used for single parts and to constrain parts.
Basic Concepts of Table Driven Parts In the manufacturing industry, you often have parts that are similar to each other except for size or a particular feature. Some examples are springs, brackets, plates, nuts, and bolts. By driving part versions from an external spreadsheet, you can document a number of similar parts using one drawing. The external spreadsheet, or table, is where you make modifications to your design specifications once your drawing is set up.
Setting Up Tables A table is a spreadsheet that contains the various part versions and the values of the design variables for each version. You use Microsoft Excel to create table driven parts. First, examine the part, using the Desktop Browser. Expand the Browser by clicking the plus sign in front of TDPART1 and PART1_1. The bracket is constructed from three extrusions, three holes, and five fillets. Each feature is controlled by a design variable.
5 In the Create Table dialog box, select the desktop\tutorial folder and specify tdpart1.xls as the name of your table. Choose Save to exit the dialog box. Microsoft Excel opens a new spreadsheet containing a generic part and a value for each design variable assigned to it. Next, change the name of the generic part to 35 and add three more part versions.
3 In the Table Driven Setup dialog box, select Update Link and choose OK. Choose OK to exit the Design Variables dialog box. The Desktop Browser now contains a Table icon nested below PART1_1. The four part versions you created in the spreadsheet are listed below the Table icon. The PART1_1 (35) icon displays the active version in parentheses. The Table (tdpart1.xls) icon indicates the name of the spreadsheet that is linked to your drawing. Next, display each version of the table driven part.
Editing Tables Using a table to drive multiple versions of a part gives you flexibility in designing the part. You can quickly create variations of the part, and easily edit the design parameters by changing values in the cells of the spreadsheet. To add a part version to an existing table 1 Open the spreadsheet to edit. Browser Right-click Table (tdpart1.xls) and choose Edit. NOTE The part definition in the Browser displays the current version of the part for easy reference.
2 Add a new part version in the spreadsheet, using the values in the following illustration: 3 Save the spreadsheet and exit Microsoft Excel. 4 Update the link to the spreadsheet. Browser Right-click Table (tdpart1.xls) and choose Update. Examine the Browser. It now displays five part versions under the Table (tdpart1.xls) icon. Occasionally, errors occur when you link a spreadsheet to Mechanical Desktop.
Resolving Common Table Errors Open the file tdpart2.dwg in the desktop\tutorial folder. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40. The drawing contains a version of the simple bracket used in the previous example, but it is linked to a different spreadsheet. Before you can look for errors in the link between the drawing and the spreadsheet, you need to expand the part hierarchy.
To resolve a conflict with a linked spreadsheet 1 Resolve the conflict between the drawing and the linked spreadsheet. Browser Right-click Table (tdpart.xls) and choose Resolve Conflict. An AutoCAD message dialog box is displayed asking if you would like to update the table. 2 In the message dialog box, choose Yes. The HD variable controls the diameters of the holes for the bracket. The first part version is missing an entry in cell B10. 3 In cell B10, enter .1875.
To display the first part version 1 Display the first part version. Browser Double-click the 35 icon nested under PART1_1. The 35 angle bracket is recalculated from the values in the table and then displayed. 2 Repeat step 1 for the remaining four part versions. Save your file. Next, you suppress features for some of the part versions in your table. The smaller brackets do not require the brace, so you will suppress the features associated with it for those versions.
To suppress a feature 1 Display the first part version. Browser Double-click the 35 icon nested under PART1_1. 2 Use AMSUPPRESSFEAT to suppress the brace feature, responding to the prompt. Browser Right-click Brace and choose Suppress. The highlighted features will be suppressed. Continue? [Yes/No] : Press ENTER The brace feature is suppressed and is no longer visible on your screen. The bracecut feature and four fillets are dependent on the brace feature, so they are also suppressed.
To append a suppressed feature to a table 1 Use AMVARS to append the suppressed features to the spreadsheet. Desktop Menu Part ➤ Design Variables 2 In the Design Variables dialog box, under Table Driven, choose Setup. 3 In the Table Driven Setup dialog box, specify: Type: Both Format: Concatenate Tables Choose Append. Microsoft Excel spreadsheet tdpart2.xls is displayed. A new entry, brace, has been added under the existing design variables.
To create a suppressed feature in a table 1 In the spreadsheet, in cell A13 enter bracecut. 2 In cell F13 enter S. 3 Save the spreadsheet and exit Microsoft Excel. 4 Choose OK to exit the Table Driven Setup dialog box without updating the link. 5 Choose OK to exit the Design Variables dialog box. You have created two table driven suppressed features. To activate the table driven suppression of these features, you update the link to the table.
To manually unsuppress a feature 1 Use AMUNSUPPRESSFEAT to unsuppress the brace feature. Browser Right-click Brace and choose Unsuppress+. NOTE By using Unsuppress+ in the Browser, you unsuppress the feature you select and all dependent features. If you use the Browser, the dialog box is not displayed. 2 If you use the Unsuppress By Type dialog box, verify that Fillets, which are the dependent features, and Extrudes are selected. Choose OK. The brace and its dependent features are unsuppressed.
To display a part version 1 Display the part. Browser Double-click the 35 icon nested below Table (tdpart2.xls). The part is recalculated using the values for the 35 version in the linked table. In the Browser, the suppressed features are grayed out. 35 version 2 Repeat step 1 for the 46 version. The brace and its dependent features in this version are suppressed. 3 Repeat step 1 for the 57 and 69 versions. Note that the features are not suppressed in these versions.
Working with Two Part Versions You can create copies of a part and work with different versions to create assemblies. In this lesson, you copy a part and display two versions simultaneously. To copy a part definition 1 Display the 35 version of the bracket. Browser Double-click the 35 icon nested below Table (tdpart2.xls). 2 Use UCS to return to the World Coordinate System so that the copy of the part is oriented the same as the original.
6 In the Copy Definition dialog box, specify: New Definition Name: Enter part2 Choose OK. 7 Continue on the command line. Specify new insertion point: Specify a point to the right of the existing part Specify insertion point for another instance or : Press ENTER copied part definition Choose OK to close the Assembly Catalog dialog box. The Browser now contains a PART2_1 definition. Because you copied the original part definition, its relationship to the spreadsheet, tdpart2.
To display a different version 1 Use AMACTIVATE to activate PART2_1. Browser In the Browser, right-click PART2_1 and choose Activate Part. 2 Display the 57 version for PART2_1. Browser Double-click the 57 icon nested under PART2_1. The 57 version of PART2_1 is displayed. PART2_1 Save your file. Next, you set up the drawing for plotting.
To create a base view 1 Use the Browser to turn off the visibility of PART1_1. Browser Right-click PART1_1 and choose Visible. 2 Use AMMODE to switch to Drawing mode. Browser Select the Drawing tab. Mechanical Desktop switches to Drawing mode. A title block has been inserted into the drawing. 3 Use AMDWGVIEW to create the base view. Context Menu In the graphics area, right-click and choose New View.
1 2 4 Continue on the command line to place the base view. Specify location of base view: Specify a point in the top center of the title block Specify location of base view: Press ENTER Your drawing should look like this. Next, create side and bottom orthographic views of the part.
To create an orthographic view 1 Create the orthographic view. Context Menu In the graphics area, right-click and choose New View. 2 In the Create Drawing View dialog box, select the view type Ortho. On the Hidden Lines tab, specify: Display As: Wireframe Choose OK.
5 In the Create Drawing View dialog box, select the view type Ortho. On the Hidden Lines tab, specify: Display As: Wireframe Choose OK. 6 On the command line, respond to the prompts as follows: Select parent view: Pick a point inside the base view Specify location for orthogonal view: Specify a point below the base view Specify location for orthogonal view: Press ENTER Your drawing should look like this. Save your file. Look at the Browser. There are two ortho views and a base view.
Cleaning Up the Drawing To clean up the drawing, you change the parametric dimensions to be displayed as parameters, hide extraneous dimensions, and move dimensions for clarity. NOTE For detailed cleanup instructions see “Cleaning Up Drawings” on page 322 in chapter 13. Displaying Dimensions as Parameters The parametric dimensions used to define a part are displayed with the values for the active version of the part.
Your drawing should look like this. Next, hide the extraneous dimensions. Hiding Extraneous Dimensions When drawing views are created, Mechanical Desktop displays all the parametric dimensions that are related to the part display in each view. Usually, some cleanup is required because of overlapping or redundant dimensions.
To hide an extraneous dimension in a base view 1 Use AMVISIBLE to hide extraneous dimensions. Desktop Menu Drawing ➤ Drawing Visibility In the Desktop Visibility dialog box, choose Select. NOTE If you choose the toolbutton method to hide the dimensions, the Desktop Visibility dialog box is not displayed. Select the dimensions to hide. Use Zoom Realtime while selecting the dimensions.
To hide a dimension in an orthographic view 1 Use AMVISIBLE to hide dimensions. Desktop Menu Drawing ➤ Drawing Visibility 2 In the Desktop Visibility dialog box, choose Select. NOTE If you choose the toolbutton method to hide the dimensions, the Desktop Visibility dialog box is not displayed. Select the dimensions to hide. 3 In the side ortho view, hide the db dimension, the two db/2 dimensions, and the db/4 dimension. You do not need to hide dimensions in the bottom ortho view.
To move a dimension 1 Use AMMOVEDIM to move the parametric dimensions in the base view, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Dimensions ➤ Move Dimension.
2 Continue moving dimensions until your base view looks like this. 3 Move the dimensions in the ortho views. The ortho views should look like this. side view bottom view Next, add reference dimensions, to fully define the part.
Enhancing Drawings To finalize the presentation of the drawing, you add power dimensions, displayed as parameters and create a hole note to describe the three holes in the bracket. Creating Power Dimensions The drawing views are intended to display the generic part. When you display parametric dimensions using design variables, and you power dimension your drawing views, the views represent the generic part.
3 1 2 2 In the Power Dimensioning dialog box, change the default text to tb/2. Choose OK.
3 Continue on the command line to add a power dimension to the fillet at the bottom of the long leg: (Single) Specify first extension line origin or [Angular/Options/Baseline/Chain/ Update]
Your drawing should resemble the following illustration. 6 Place power dimensions so that the orthographic views look like this. Next, create a hole note that describes the three holes in the bracket. Creating Hole Notes Mechanical Desktop provides a tool for creating hole notes, which saves you time when annotating your drawing. In the side view, create a hole note for one of the holes in the long leg of the bracket.
To create a hole note 1 Use AMNOTE to create the hole note, responding to the prompts. Context Menu In the graphics area, right-click and choose Annotation ➤ Hole Note. Select object to attach [rEorganize]: Specify the upper hole in the long leg of the bracket (1) Next Point : Specify the location (2) and press ENTER. 1 2 2 In the Note Symbol dialog box, select the Leader tab. In Leader Justification, specify Middle of All Text. Choose OK. The hole note is displayed in your drawing.
Edit the hole note so that it is typical for all three holes. 3 Use AMPOWEREDIT to edit the hole note, responding to the prompt. Context Menu Select the hole note, then right-click the note and choose Edit. 4 In the Note Symbol dialog box, select the Note tab, and change the text to read as follows: %%c hd THRU (typ of 3) Choose OK. The side view should now look like this. Save your file. Now that the power dimensions and annotations are in place, paste the linked spreadsheet into the drawing.
Pasting Linked Spreadsheets Pasting a linked spreadsheet into a drawing provides more flexibility for working with the table that defines the values for the part versions. The external spreadsheet can be opened and modified while you are working, and the results are reflected in the drawing. To paste a linked spreadsheet into a drawing 1 Use AMMODE to return to the Part/Assembly environment. Browser Select the Model tab. 2 Open the spreadsheet. Browser Right-click Table (tdpart2.xls) and choose Edit.
6 Paste the selected area of the spreadsheet into the drawing. Desktop Menu Edit ➤ Paste Special 7 In the Paste Special dialog box, choose Paste Link. 8 Place the selected cells in the drawing. Your drawing should look like this. NOTE Depending on the zoom factor of your display at the time you paste the image, you may have to resize it. Select the image, and use a corner grip to resize it to fit in the drawing. Save your file.
398
Assembling Parts 16 In This Chapter You can build part assembly models from two or more ■ Using external parts in an assembly parts, or parts grouped in subassemblies. Like part features, parts and subassemblies act as building blocks. Autodesk® Mechanical Desktop® builds individual parts ■ Using assembly constraints ■ Analyzing the assembly ■ Creating assembly scenes ■ Using assembly tweaks and trails and subassemblies into an assembly.
Key Terms Term Definition 3D constraint In assembly modeling, an associative link between two or more parts that controls their locations relative to each other and to their placement within the assembly. Assembly Catalog The means of attaching and cataloging local and external parts and subassemblies in the Assembly Modeling environment. Use the All and External tabs to specify contents, which can be instanced, copied, renamed, replaced, externalized, removed, localized, sorted, unloaded, and reloaded.
Basic Concepts of Assembling Parts You create assemblies from parts, either combined individually or grouped in subassemblies. Mechanical Desktop builds these individual parts and subassemblies into an assembly in a hierarchical manner according to relationships defined by constraints. Using the Desktop Browser, you can restructure the hierarchy of an assembly as needed, while retaining the design constraints. See “Using the Desktop Browser” on page 414.
Starting Assembly Designs An assembly design might begin as an overall conceptual design. You may know how the parts are assembled but you may not know all the details about each part. Before you begin, decide how you want to lay out your assembly. ■ ■ ■ Start with a design idea. Decide whether you need to create new parts, or if you can use existing parts. Start drawing the parts.
Using External Parts in Assemblies The parts that make up the assembly model can be created and maintained in other files. These parts are called externally referenced parts. When a part changes, all instances of that part in other files are automatically updated. Using parts from other files as external references is similar to external referencing (xref) in AutoCAD. Because they are external, you can reuse referenced parts in future assemblies.
A Browse for Folder dialog box lists your network connections and directories. 3 In the Browse for Folder dialog box, specify the desktop\tutorial folder to be your working directory. Choose OK. NOTE If you have installed Mechanical Desktop in a different location, browse through your directories to locate the correct folder. All drawing files in the desktop\tutorial folder are listed under Part and Subassembly Definitions on the External tab. 4 In the desktop\tutorial folder, double-click the PLIERT defin
Notice that each of the external files is preceded by an icon, indicating whether it is a part or assembly file. 5 Attach and instance the HEXNUT and HEXBOLT parts to the current assembly. plierb pliert hexbolt hexnut As you instance each part, you return to the Assembly Catalog. In the Part and Subassembly Definitions list, each attached part is displayed on a white background. When all parts are instanced into the assembly, choose OK. Examine the Browser.
Assembling Parts After parts or subassemblies have been created, you apply constraints to position them relative to one another. Each time you apply a constraint to a part, you eliminate some degrees of freedom (DOF). The number of degrees of freedom determines the movement of a part in any direction; the more constraints applied, the less the part can move. A degrees of freedom symbol illustrates the instance order of the parts and how the parts can move.
Constraining Parts Use a mate constraint to join the PLIERT and HEXBOLT parts. Zoom in as needed to make the selection easier. To add a mate constraint between parts 1 Use AMMATE to select the first set of geometry, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
The corresponding faces of the HEXBOLT and PLIERT parts are mate constrained. mated planes NOTE The DOF symbol is useful during constraining but has been turned off for clarity in the illustrations. 3 Use AMMATE to constrain HEXBOLT to the bolt hole on PLIERT along their axes, following the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
In addition to a mate constraint on the faces of the bolt head and pliers, the HEXBOLT and the PLIERT bolt hole are constrained along their axes. 4 Examine the DOF symbol. It should show that only the rotational degree of freedom remains unsolved. In this case, it does not need to be solved. You could use the insert constraint to solve the same degrees of freedom as the two mate constraints.
To mate to a grounded part 1 Turn on the DOF symbol for PLIERB. Browser Right-click PLIERB_1 and choose DOF Symbol. The DOF symbol is represented by a number within a circle, indicating that it has no degrees of freedom. Because it is the first part created in the assembly drawing, PLIERB becomes the grounded part. As you apply assembly constraints, the grounded part remains stationary. If you move the grounded part, all parts constrained to it also move.
The two parts of the pliers body are now plane mated on corresponding faces. mated planes To mate parts on their axes 1 Mate the HEXBOLT part to the PLIERB part along their axes, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
2 Mate the HEXNUT to the face of the pliers, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
4 Mate the nut to the bolt along their axes to pass the bolt through the hole. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate. Select first set of geometry: Select the bolt hole on HEXNUT (11) First set = Axis, (arc) Select first set or [Clear/fAce/Point/cYcle] : Press ENTER Select second set of geometry: Select the bolt hole on PLIERB (12) Second set = Axis, (arc) Select second set or [Clear/fAce/Point/cYcle] : Press ENTER Enter offset <0.
Using the Desktop Browser As you assemble parts, a graphical hierarchy of the assembly is illustrated in the Desktop Browser. Each 3D constraint applied to an assembly component is listed below the component. You can tell at a glance which constraints exist between which components, because the other component to which the constraint applies is shown in the hierarchy. When you hold the cursor over a constraint, feature, or tweak in the Browser, a tooltip displays pertinent data.
4 In the Edit 3D Constraint dialog box, change the offset to 0.05. Click the Update icon. You can see the hexbolt offset the new distance. Experiment with changing the offset again, using the Update icon to see the change. Choose Cancel. The original offset distance of 0.00 remains in effect. You can easily edit values and see them take effect without permanently changing your assembly.
To change the color of a part with the Browser 1 Activate HEXBOLT_1. Browser Right-click HEXBOLT_1 and choose Activate Part. 2 Open the Select Color dialog box to change the color of HEXBOLT_1. Browser Right-click HEXBOLT_1 and choose Properties ➤ Color. 3 In the Select Color dialog box, select Red, and then choose OK. This color applies to all instances of HEXBOLT. 4 Activate the assembly to view the changed color Browser Right-click S_PLIER and choose Activate Assembly.
To localize an external part with the Browser 1 Localize the external parts HEXBOLT_1 and HEXBOLT_3. Browser Press CTRL and select HEXBOLT_1 and HEXBOLT_3. Right-click the selected parts and choose All Instances ➤ Localize. This shortcut method enables you to localize and externalize parts without opening the Assembly Catalog. When you select a local part in the Browser, the externalize option is available.
To check for interference 1 Change to one viewport. Command 1 2 Change to the right isometric view. View ➤ 3D Views ➤ Front Right Isometric Desktop Menu 3 Use AMINTERFERE to check for interference, responding to the prompts. In the graphics area, right-click and choose Analysis ➤ Check Interference.
To calculate mass properties 1 Use AMASSMPROP to select the parts for the mass properties calculation, following the prompts, and open the Assembly Mass Properties dialog box. Context Menu In the graphics area, right-click and choose Analysis ➤ Mass Properties.
3 Select the Results tab. The results window for PLIERB remains empty until you calculate the results. 4 Choose Calculate. Message dialogs appear warning that density is not specified for the other parts in the assembly. Choose OK to proceed. Mass properties are calculated according to the values you set. Choose Done. NOTE You can save mass properties calculations to a file to use in design analysis, and you can export the results. Next, you create scenes of the assembly.
Assembly trails indicate the path of the assembly explosion. With the exception of the grounded part, assembly trails can be created for all parts. When you create assembly trails, a new layer is automatically created for them. You can automatically create trails when you create tweaks. First, you set an explosion factor and then create an exploded assembly scene. Then you add trails to show how parts are assembled. From a scene, you create drawing views.
Next, align the exploded parts in the assembly scene. You can tweak the position and orientation of individual parts or rotate them for better visibility. In the Browser, verify that the Scene tab is selected. Unless the scene is activated, you cannot tweak parts to adjust their position or add trails to show how they are assembled. To align scene parts 1 Use AMTWEAK to move the HEXNUT part closer to the other parts, responding to the prompt.
1 The HEXNUT position is tweaked by the specified distance. NOTE The grounded part of an assembly or subassembly cannot be tweaked. Its position is fixed. 4 Use AMTRAIL to show the direction of the explosion and tweak paths, responding to the prompt. Context Menu In the graphics area, right-click and choose New Trail.
5 In the Trail Offsets dialog box, specify: Offset at Current Position: Distance: Enter 1 Over Shoot: Select the option Offset at Assembled Position: Distance: Enter 1 Over Shoot: Select the option Choose OK. The assembly trail for HEXBOLT is displayed. 6 Apply assembly trails to the PLIERB and HEXNUT parts, responding to the prompt. Context Menu In the graphics area, right-click and choose New Trail.
2 7 In the Trail Offsets dialog box, specify: Offset at Current Position: Distance: Enter 1 Over Shoot: Select the option Offset at Assembled Position: Distance: Enter 1 Over Shoot: Select the option Choose OK. The assembly drawing automatically updates the current scene to reflect the tweaks and assembly trails. Save your file. Choose OK in the External Part Save dialog box to bring all parts up to date. Next, you create drawing views of the assembly scene.
To add a custom paper size to a plotter setup 1 Use AMMODE to switch to Drawing mode. Browser Choose the Drawing tab. 2 Add a custom paper size to an existing plotter. Browser Right-click Layout1 and choose Page Setup. 3 In the Page Setup dialog box, select the Plot Device tab and specify: Name: DWF Classic.
4 Choose Properties. 5 In the Plotter Configuration Editor dialog box, expand User-Defined Paper Sizes and Calibration. Select Custom Paper Sizes and choose Add. 6 Use the Custom Paper Size Wizard to define a paper size of 18 x 12 inches with no indents. Choose Next until the setup is finished. 7 Save your changes to the DWF Classic.pc3 file. Next, you set up the drawing layout and insert a title block.
To set up a drawing layout 1 In the Page Setup dialog box, select the Layout Settings tab and specify: Paper Size: User 1 (18.00 x 12.00 inches) Plot Scale: 1:1 Choose OK. 2 Use MVSETUP to insert a title block. Browser Right-click Layout1 and choose Insert Title Block. In the AutoCAD text window, respond to the prompt as follows: Enter number of title block to load or [Add/Delete/Redisplay]: Enter 8 3 Continue on the command line. Create a drawing named ansi_b.
To create a base assembly drawing view 1 Use AMDWGVIEW to create a base view. Context Menu In the graphics area, right-click and choose New View. In the Create Drawing View dialog box, specify: Type: Base Data Set: Scene: SCENE1 Choose OK.
The base drawing view is displayed. Next, create an isometric view of the assembly. To create an isometric assembly drawing view 1 Create an isometric view. Context Menu In the graphics area, right-click and choose New View. In the Create Drawing View dialog box, specify: View Type: Iso In the Hidden Lines tab, specify: Calculate Hidden Lines: Choose OK.
2 Respond to the prompts as follows: Select parent view: Specify the base view Specify location for isometric view: Specify a point to place the isometric view Specify location for isometric view: Specify another point or press ENTER Examine the Browser. The views are nested under a Scene icon which is nested under Layout1. Save your file. Now you can add reference dimensions, which can be moved, frozen, and thawed in each drawing view.
To add a reference dimension 1 Zoom in to enlarge the area you want to dimension. Context Menu In the graphics area, right-click and choose Zoom. 2 Use AMREFDIM to add a reference dimension, following the prompts. Context Menu In the graphics area, right-click and choose Reference Dimension.
Editing Assemblies Design or specification changes require most assembly designs to be documented and edited frequently. You modify parts, rearrange parts and features in the hierarchy of the assembly tree, and change or delete constraints. Because the parts and assembly are parametric, changes are fast and updates are immediate. Editing an external part definition automatically changes the assembly model wherever the part is instanced.
Editing External Parts To update all instances of a part in assemblies, you need to edit the original part. You alter part features by changing dimensions, changing the constraints, or adding new features. The changes take effect in the assembly. In this tutorial, you edit the external PLIERT part from within your assembly drawing. This is called editing in place. In the following steps, you add another hole to the PLIERT part, and modify assembly constraints.
4 Zoom in on PLIERT. 5 Use AMSKPLN to create a new sketch plane, responding to the prompts. Context Menu In the graphics area, right-click and choose New Sketch Plane.
To create a new feature on an external part 1 Use CIRCLE to place a new hole, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Circle. CIRCLE Specify center point for circle or [3P/2P/Ttr (tan tan radius)]: Select a point near the existing hole Specify radius of circle or [Diameter]: Draw a circle approximately the same size as the other hole 2 Use AMPROFILE to solve the sketch.
Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Select the circle (1) Select second object or place dimension: Specify a point for the location of the dimension (2) Enter dimension value or [Undo/Radius/Ordinate/Placement point] <0.2003>: Enter .22 Solved underconstrained sketch requiring 2 dimensions or constraints.
Choose OK to exit the dialog box. The new hole is extruded, and its position is constrained to the original hole. Save your file. 5 The External Part Save dialog box indicates a change in the PLIERT drawing. Choose OK to save the changes you have made. new bolt hole The Browser returns to normal. The inactive parts are no longer dimmed, and the assembly reflects the new PLIERT part.
To delete an assembly constraint 1 In the Desktop Browser, click the plus sign on PLIERB_1 to expand the hierarchy. Select the Assembly filter at the bottom of the Browser to filter out all information except the assembly constraints. 2 In the Browser, click the plus sign on HEXBOLT_1 to expand the hierarchy. Right-click the Mate ln/ln constraint of HEXBOLT_1, and choose Delete. 3 Delete the Mate pl/pl constraints of HEXBOLT_1. 4 Delete constraints for PLIERB, PLIERT, and HEXNUT.
To apply an assembly constraint 1 Use AMINSERT to constrain PLIERT_1 and HEXBOLT_1, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert.
2 Use AMINSERT to constrain PLIERB and PLIERT, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert.
Move parts so you can easily see selection points. Select first circular edge: Select the bolt hole on PLIERB (5) First set = Plane/Axis Enter an option [Clear/Flip] : Flip the direction arrow toward HEXNUT and press ENTER Select second circular edge: Select the hole on HEXNUT (6) Second set = Plane/Axis Enter an option [Clear/Flip] : Flip the direction arrow toward PLIERB and press ENTER Enter offset <0.
Combining Parts In This Chapter This Autodesk® Mechanical Desktop® tutorial builds on the part and assembly modeling techniques that you 17 ■ Working in Single Part mode ■ Changing part definitions ■ Combining and intersecting learned in previous chapters.
Key Terms Term Definition base part The active part where toolbody parts are aligned and subsequently combined. Boolean modeling A solid modeling technique in which two solids are combined to form one resulting solid. Boolean operations include cut, join, and intersect. Cut subtracts the volume of one solid from the other. Join unites two solid volumes. Intersect leaves only the volume shared by the two solids.
Basic Concepts of Combining Parts In Mechanical Desktop® the parametric Boolean capabilities for combining parts provide a combination of modeling flexibility and convenience. To combine two parts, you identify which part you want to use as the base part and make it active. Then, you position the toolbody part on the base part, using the MOVE or ROTATE command or assembly constraints. You use AMCOMBINE to cut, join, or intersect the toolbody part with the base part.
In the following illustration, the appearance of the part is the same, whether or not you nest the toolbodies, but the part displayed in the Desktop Browser on the left is easier to manage and has a less cumbersome display than the one in the Browser on the right. To edit CAM_1, on the left, you need to expose only one toolbody. Nested toolbody parts, like those in the example on the right, usually have more complex constraint systems and require multiple part updates after modification.
Creating Parts In this tutorial, you create a chassis suspension component for an off-road recreational vehicle. The part is an axle spacer. You create most of the features of this part by first creating the basic shape. Then, you create separate parts that you use as tools to add additional features to the basic shape. Open the file spacer.dwg in the desktop\tutorial folder. This drawing contains a fully constrained profile sketch of the basic shape of the axle spacer.
5 Use VIEW to change your viewpoint to a previously saved view. Desktop Menu View ➤ Named Views In the View dialog box, select SPACER_VIEW, and choose Set Current. Choose OK. 6 Use AMEXTRUDE to extrude the profile. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Distance: Enter 64 Draft Angle: Enter -2 Termination: Type: MidPlane Choose OK.
2 Use HIDE to hide the silhouette edges. Desktop Menu View ➤ Hide The spacer has a boss at the bottom and a relief at the top. Next, you use two part definitions to construct the toolbody parts. You combine those toolbody parts with the spacer to create the boss and relief. Creating Toolbody Part Definitions The shapes of the new toolbody parts are similar to the shape of the spacer profile. The easiest way to create the toolbodies is to use copies of the spacer to construct the new toolbody parts.
Because you are working in the Part Modeling environment, Mechanical Desktop filters the part and assembly drawings in your working directory and lists only the part files. A thumbnail preview of the part icon precedes the drawing name. If a part file does not contain features, it is preceded by a red AutoCAD icon. 4 In the Part Catalog, right-click BOSS and choose Attach.
The Part Catalog is displayed. 6 Choose the All tab. The boss toolbody is listed in External Toolbody Definitions. Choose OK. Next, localize and make a copy of the boss toolbody, to create a definition for the relief toolbody using the Browser shortcut methods. To localize an external toolbody and copy its definition 1 Localize external toolbody BOSS_1. Browser Right-click BOSS_1, and choose All Instances ➤ Localize. The boss toolbody is localized.
4 The Copy Definition dialog box is displayed. In New Definition Name , enter relief. Choose OK. 5 Position the instance of the relief toolbody definition to the right of the boss toolbody, and press ENTER. The new relief toolbody definition is listed under Local Toolbody Definitions in the Part Catalog. Choose OK. Examine the Browser. It contains one part and two unconsumed toolbodies. Save your file.
The boss toolbody on the completed spacer follows the profile of the spacer, but its corners are rounded. The next step is to combine a cylinder with the boss toolbody. boss In the Browser, right-click BOSS_1 and choose Activate Toolbody. Right-click BOSS_1 again, and choose Zoom To. To create a cylinder toolbody to combine with the boss toolbody 1 Use AMNEW to create a new toolbody definition, responding to the prompts. Context Menu In the graphics area, right-click and choose Toolbody ➤ New Toolbody.
5 Select the circle, and enter a dimension of 86. 6 Use AMEXTRUDE to extrude the profile. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Distance: Enter 5 Draft Angle: Enter 2 Termination: Type: Blind Choose OK. Next, you use assembly constraints to position the cylinder at the bottom of the BOSS_1 toolbody. Then you use a Boolean intersect operation to combine the two parts.
1 Select second set of geometry: Select the arc (2) Second set = Axis, (arc) Select second set or [Clear/fAce/Point/cYcle] : Enter p Second set = Point, (arc) Select second set or [Clear/aXis/fAce/cYcle] : Select the arc (3) Second set = Plane, (arc) Enter an option [Clear/aXis/Flip/cYcle] : Enter x Second set = Axis, (arc) Select first set or [Clear/fAce/Midpoint/cYcle] : Enter m Second set = Axis, (arc) Select first set or [Clear/fAce/Midpoint/cYcle] : Press ENTER
2 Use MOVE to move the cylinder for easier selection, responding to the prompts. Context Menu In the graphics area, right-click and choose Part Menu ➤ 2D Sketching ➤ Move. Select objects: Specify the cylinder Select objects: Press ENTER Base point or displacement: Specify a point Second point of displacement: Specify a second point and press ENTER 3 Create the second mate-line constraint, responding to the prompts.
The center of the cylinder is aligned with the line between the two boss arc centers. Together, the two mate constraints position the cylinder at the bottom of the boss. The center of the cylinder is coincident with the center of the boss. Now, you are ready to combine the boss toolbody with the cylinder. Because the boss toolbody will be the base part in the Boolean operation, you need to make it active. To create a combine feature 1 Use AMACTIVATE to activate BOSS_1.
Working with Combine Features The Desktop Browser now shows that the boss toolbody has a combine feature. The boss cylinder is a toolbody in the combine feature. The next step is to constrain and combine the boss toolbody with the spacer. To constrain and combine a toolbody to the base part 1 Use AMACTIVATE to activate the SPACER. Browser In the Browser, right-click SPACER and choose Activate Part. 2 Use AMMATE to apply a mate constraint to the boss toolbody and the spacer, responding to the prompts.
1 2 Select second set of geometry: Select the bottom right edge of the spacer (3) Second set = Axis, (arc) Select second set or [Clear/fAce/Point/cYcle] : Enter p Second set = Point, (arc) Select second set or [Clear/aXis/fAce/cYcle] : Select the opposite edge of the spacer (4) Second set = Plane, (arc) Enter an option [Clear/aXis/Flip/cYcle] : Enter x Second set = Axis, (arc) Select second set or [Clear/fAce/Midpoint/cYcle] : Press ENTER Enter offset <0>: Press ENTER 3 4
The boss toolbody is now aligned with the spacer. 4 Use AMCOMBINE to combine the spacer and the boss toolbody, responding to the prompts. Context Menu In the graphics area, right-click and choose Part Menu ➤ Placed Features ➤ Combine. Enter parametric boolean operation [Cut/Intersect/Join] : Enter j Select part (toolbody) to be joined: Select the boss toolbody Save your file.
Creating Relief Toolbodies The Desktop Browser now shows a nested toolbody construction. The boss cylinder toolbody is a combine feature of the boss toolbody, and the boss toolbody is a combine feature of the spacer. Next, you create the relief toolbody, to cut material from the spacer. In the Browser, right-click RELIEF_1 and choose Zoom To. To add a new toolbody name in the Browser 1 Use AMNEW to create a new toolbody called RELIEF_CYLINDER, responding to the prompts.
To create a new part 1 Use CIRCLE to draw a circle near RELIEF_1. Context Menu In the graphics area, right-click and choose Part Menu ➤ 2D Sketching ➤ Circle. 2 Use AMPROFILE to create a profile from the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. 3 Use AMPARDIM to constrain the profile. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select the circle, and enter a dimension of 90.
2 After adding the constraints, use AMACTIVATE to activate RELIEF_1. Browser In the Browser, right-click RELIEF_1 and choose Activate Toolbody. 3 Combine the relief cylinder and the relief toolbody. Context Menu In the graphics area, right-click and choose Part Menu ➤ Placed Features ➤ Combine. 4 Choose Intersect, and select the relief cylinder as the toolbody. Save your file.
To combine a relief toolbody with a spacer 1 Use AMMATE for assembly constraints just as you did to align the relief toolbody with the spacer. Desktop Menu Toolbody ➤ 3D Constraints ➤ Mate. When you combine the spacer and the relief toolbody in step 3, you will cut the spacer with the toolbody. Therefore, be sure to align the top of the toolbody with the top of the spacer.
Adding Weight Reduction Holes The axle spacer is a high-performance chassis component, so its weight must be kept to a minimum. To achieve this, you cut weight reduction holes into the part. The manufacturer of the part offers several size spacers with different size weight reduction holes. The use of parametric Boolean operations is an ideal way to model the part, because it is easy to replace one combine feature with another. The file spacer.
4 Align the axis of one of the reduction extrusion cylinders with a line that runs through the center points of the spacer arcs. Use the point option when you define the axis, as you did with previous mate constraints. 5 Use another mate constraint to align the axis of the adjacent weight reduction extrusion cylinder with a line that runs through the center points of the spacer arcs. 6 Make sure that the spacer is the active part, and use AMCOMBINE to combine the two parts.
The weight reduction holes are very close to the relief cut. For balance, the holes must remain centered in the spacer. To provide enough material between the holes and the relief, you need to reduce the depth of the relief and the diameter of the holes. To make the change, you edit the nested relief cylinder toolbody and reduce its extrusion distance.
Mechanical Desktop recovers the toolbody and displays it in its constrained position on the spacer. The relief toolbody is active, and it contains the relief cylinder toolbody. 3 Use AMEDITFEAT to recover the relief cylinder, responding to the prompt. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit.
1 In the Browser, note that the relief toolbody and the relief cylinder toolbody have yellow backgrounds. This indicates that they need to be updated. 7 Use AMUPDATE to update the parts, responding to the prompts. Context Menu In the graphics area, right-click and choose Update Full. Toolbody Updates Pending: 2 Enter an option [Full/stEp/posiTioning] : Press ENTER to update both parts Next, you change the diameter of the weight reduction holes.
To edit the weight reduction cylinders 1 In the Browser, right-click WR_HOLES_1 and choose Open to Edit. Mechanical Desktop opens the external file containing the weight reduction holes. 2 Expand WR_HOLES in the Browser. 3 Right-click ExtrusionMidplane1 and choose Edit. 4 Choose OK to exit the Extrusion dialog box. 5 Continue on the command line. Select object: Specify the diameter dimension Enter dimension value <42>: Enter 35 Solved fully constrained sketch.
Adding Weight Reduction Extrusions One more weight reduction extrusion remains. The geometry for the sketch is stored on the WEIGHT_REDUCTION_EXTRUSION layer. To copy a sketch to create a new sketch 1 Return to wireframe display. Desktop Menu View ➤ Shade ➤ 2D Wireframe, and then View ➤ Regen 2 Use LAYER to turn on the WEIGHT_REDUCTION_EXTRUSION layer and make it current.
6 Turn off LAYER 0, which contains the spacer. Desktop Menu Assist ➤ Format ➤ Layer 7 Use AMPROFILE to profile the sketch. Context Menu In the graphics area, right-click and choose Part Menu ➤ Sketch Solving ➤ Profile. 8 Select the sketch and all of its existing dimensions. Mechanical Desktop converts the standard dimensions to parametric dimensions and solves the sketch. Solved underconstrained sketch requiring 2 dimensions or constraints.
Valid selections: line, arc, circle or spline segment Select object to be reoriented: Select the arc (3) Valid selections: line, arc, circle or spline segment Select object x value is based on: Select the arc (4) Solved fully constrained sketch. Valid selections: line, arc, circle or spline segment Select object to be reoriented: Press ENTER Enter an option [Hor/Ver/PErp/PAr/Tan/CL/CN/PRoj/Join/XValue/YValue/Radius/Length/Mir/Fix/ eXit] : Press ENTER 2 Use VIEW to restore the saved view.
To combine a weight reduction extrusion with a spacer 1 Turn on LAYER 0, and make it current. Desktop Menu Assist ➤ Format ➤ Layer 2 Activate the spacer, and then combine the weight reduction extrusion and the spacer. Context Menu In the graphics area, right-click and choose Placed Features ➤ Combine. 3 Choose Cut, to cut the weight reduction extrusion from the spacer, and then select the weight reduction extrusion as the toolbody. 4 Remove the hidden lines. Desktop Menu View ➤ Hide Save your file.
In the Hole dialog box, specify: Operation: Drilled Termination: Through Placement: Concentric Hole Parameter: Size: 12 3 Respond to the prompts as follows: Select work plane, planar face, or [worldXy/worldYz/worldZx/Ucs]: Select the top face (1) Select concentric edge: Select the cylindrical edge (2) 1 2 4 Repeat steps 2 and 3 to create three more holes, and then press ENTER.
5 Use HIDE to remove the hidden lines. Desktop Menu View ➤ Hide The spacer contains one extrusion, four combine features, and four holes. Save your file. You have now created and edited a combined part in the Part Modeling environment.
Assembling Complex Models In This Chapter In a previous Autodesk® Mechanical Desktop® tutorial, you created a simple assembly. In this tutorial, you create a more complex assembly that includes a subassembly. You work with contraints, external parts, and part instances.
Key Terms Term Definition base view The first drawing view you create. Other drawing views are derived from this view. bill of material database A dynamic database containing a list of all the parts in an assembly. Used to generate parts lists that contain associated attributes such as part number, manufacturer, and quantity. exploded view Separates parts and subassemblies to show how they fit together. Automatically updated if the assembly or one of its parts changes.
Basic Concepts of Complex Assemblies Assemblies can consist of any number of externally referenced and local parts. You can also have any number of subassemblies, both local and externally referenced. The advantage to having externally referenced parts and subassemblies is that you can use the files in any number of assembly files. In complex assemblies, the same part is often used in multiple locations. Each part definition defines a unique part.
In this lesson, the model is organized and assembled in a particular order. The assembly contains existing parts and referenced external files. A new plate design is also referenced into the current file as part of a subassembly. Open the file pullyasm.dwg in the desktop\tutorial folder. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
In the Desktop Browser, click the plus sign next to PULLYASM. The assembly tree expands to reveal the part files in the order in which they were added, or referenced, into the file pullyasm.dwg. In the Browser, each part is followed by a number that indicates the order in which it was instanced. In this case, each part has only one instance. As you add more instances, each one will be numbered incrementally. Icons with a teal background are externally referenced parts.
To localize a part 1 Localize the PULLEY4, BUSHING, and SHAFT parts. Browser Press CRTL and select PULLEY4, BUSHING, and SHAFT. Right-click PULLEY4 and choose All Instances ➤ Localize. In the Browser, note that the PULLEY4, BUSHING, and SHAFT icons no longer have a teal background, which indicates that the externally referenced Mechanical Desktop® parts are now local parts. Links to the external files are severed. Any changes made to these parts affect only the instances in the current assembly.
To reference an external part 1 Use AMCATALOG to reference an external part. Context Menu In the graphics area, right-click and choose Catalog. In the Assembly Catalog, choose the External tab. 2 In Directories, right-click and choose Add Directory. Select the desktop\tutorial folder, and choose OK. All the part and assembly files in the folder are displayed; the icon in front of each file indicates whether it is a part file or an assembly file. 3 Clear the Return to Dialog check box.
To constrain part faces along their axes using mate 1 Use AMMATE to constrain the part faces, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
You can move parts to make selection easier. The parts are automatically reassembled when you add a constraint. Or, to manually reassemble parts, set AMAUTOASSEMBLE to 0 (off). Use the Assembly Update icon in the Browser to reassemble the parts after you finish adding constraints. 2 Mate the parts on facing planes, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
To make it easier to see the constraints you have applied, select the Assembly filter in the Browser. Then, the features are hidden, and only the assembly constraints are displayed. To constrain part faces along their axes using Insert 1 Use AMINSERT to constrain the part faces along the common axes and corresponding planes, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert.
Using the insert constraint removes the same degrees of freedom as constraining planes and axes separately. This is particularly useful for bolt-inhole type constraints. The NUT2 part is constrained to BRACKET and PULLEY4 along the common axes and mating planes. 2 Constrain WASHER1 to NUT2, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert. Zoom in as needed to see the arrows that indicate the direction of insertion.
3 Constrain NUT4 to WASHER1. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert. 4 Constrain BUSHING and DPULLEY along the common axes, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert.
DPULLEY is constrained to BUSHING. To apply final mate constraints 1 Use AMMATE to constrain DPULLEY and BUSHING to BRACKET with two constraints: one to mate planes and one to mate along their axes. If you need to, refer to “To constrain part faces along their axes using mate” on page 484. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate.
2 Use AMMATE to constrain SHAFT to BRACKET along the left vertical line of the notch. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Mate. mating lines The rotational degree of freedom is removed. Save your file. The parts are assembled, and all required degrees of freedom are solved by the constraints. 3 Change to a top view and then to a right view, to verify that the parts are positioned correctly. Use the Browser to delete unwanted assembly constraints.
Creating New Parts Before you build the subassembly, you create a pulley plate part. First, you open a part file containing a constrained profile. Because you can have more than one drawing open at a time in Mechanical Desktop, you do not need to close your assembly file. In the part file, you add thickness to the profile and create additional features so that you can use it as a subassembly in your assembly. Open the file ppulley.dwg.
To extrude a sketch 1 Expand the feature hierarchy in the Browser by clicking the plus sign in front of PPULLEY_1. 2 Use AMEXTRUDE to extrude the profile. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. 3 In the Extrusion dialog box, specify: Distance: Enter 10 Choose OK to create the extrusion. To add a placed feature to a part 1 Use AMHOLE to add three drilled bolt holes to the pulley plate.
3 Continue placing two more holes concentric to the remaining arcs. Then press ENTER. The drilled holes are added and cut through the pulley plate. Later, you check for interference and modify the diameter of the holes. 4 Use AMFILLET to fillet the pulley plate edges. Context Menu In the graphics area, right-click and choose Placed Features ➤ Fillet. In the Fillet dialog box, select the Constant check box and specify: Radius: Enter 1 Return to dialog: Clear the check box Choose OK.
Creating Subassemblies You created an assembly. Now, you will create a subassembly. Each subassembly contains one or more parts or subassemblies. In the Browser, subassemblies and parts are nested under the assembly. You create, instance, and constrain parts into a subassembly just as you do into an assembly. Once the subassembly is created, it is constrained to the assembly, completing the assembly model.
The inactive PULLYASM assembly is shaded in the Desktop Browser, and the SUBPULLY subassembly is active. The active subassembly name is displayed below the command line (Target: SUBPULLY). Using External Parts Now that you have activated the new subassembly, you use external parts to create the subassembly. To attach an external part drawing as an external part 1 Use AMCATALOG to attach an external part. Context Menu In the graphics area, right-click and choose Catalog.
Notice that an attached part is indicated by a white background in the Assembly Catalog. Choose OK. Examine the Browser. The referenced parts are nested under the new subassembly hierarchy. Instancing Parts You have already attached parts to the subassembly. Each part definition is listed in the Assembly Catalog. When you instance a part in the current assembly, it refers to its part definition in the Catalog. Once a part is instanced into the subassembly, you can copy it from the Browser.
Completing Assemblies Now that the parts are instanced into the subassembly, you can complete the subassembly and constrain it to the base assembly. When the entire assembly is complete, check it for interference among parts, and obtain mass property information. NOTE The Desktop Browser shows the order in which parts and subassemblies are assembled. You can drag a part or subassembly to a different position in the Desktop Browser. Always save your file before you reorder the hierarchy.
To constrain a subassembly part 1 Use AMINSERT to constrain WASHER3 to PPULLEY, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert.
2 Constrain DPULLEY to WASHER3, responding to the prompts. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert.
3 Constrain DPULLEY3 and NUT3 to the subassembly. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert. 4 Constrain the remaining parts to finish the subassembly. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert. Save your file. Next, activate the top level of the assembly and constrain the subassembly to the top assembly.
In the Desktop Browser, the top-level assembly is no longer shaded. The active assembly name is displayed below the command line (Target: PULLYASM). completed subassembly completed root assembly 2 Move the subassembly, to make viewing easier. Then zoom in as needed to magnify selection points. Next, constrain the pulley plate subassembly to the root assembly. 3 Choose Insert to constrain the shaft of NUT2 to the pulley plate hole on the mating planes and along the common axes.
The subassembly is now constrained to the root assembly. Copy another instance of NUT3 in your drawing and constrain it to the shaft of NUT2. To add and constrain a part instance 1 Use the Browser to copy another instance of the NUT3 external part into the assembly. Browser Right-click NUT3, and choose Copy. In the graphics area, click a location for the copy, and press ENTER. 2 Constrain NUT3 to the pulley plate and the shaft of NUT2.
It is a good idea to check the position of a constrained part in another view. If the part is constrained incorrectly, use the Browser to delete the constraint. Right-click to display the menu, and choose Delete. Then move the parts as needed, and reapply the constraints. One side of the pulley assembly is complete. 3 Repeat steps 1 and 2 to copy and apply assembly constraints to WASHER3, PPULLEY, and NUT3, to complete the pulley assembly.
5 Constrain both WASHER3 parts to the DPULLEY3 parts on the pulley plate. Context Menu In the graphics area, right-click and choose 3D Constraints ➤ Insert. 6 Use Insert to constrain PPULLEY_2 to the WASHER3 parts. Constrain PPULLEY to any two instances of WASHER3, to remove the rotational degree of freedom from the pulley plate. 7 Use Insert again to constrain the NUT3 parts to the pulley plate. Save your file. The pulley assembly is complete.
In most cases, constraints are maintained with the parts and subassemblies that you move. In the event that a constraint cannot be maintained, a warning message is displayed. NOTE Instances can be lost if you restructure them up the assembly hierarchy where multiple instances of the same definition exist. Open the assembly file pullyasm.dwg from the desktop\tutorial folder, and practice using assembly restructure.
Analyzing Assemblies Next, check for interference between parts. This analysis is useful for detecting problems that may arise during the final design stages. Check each part for interference. If any interference is detected between parts, interference solids can be created to illustrate where the interference occurs. To check for interference 1 Use AMINTERFERE to check for interference. Context Menu In the graphics area, right-click and choose Analysis ➤ Check Interference. Respond to the prompts.
1 2 You should detect two examples of interference. Both DPULLEY and WASHER3 parts interfere with the holes on PPULLEY. The drilled holes in the pulley plate are too small. The pulley plate is an external part, but it can be edited from within the assembly file. If you are working in a very large assembly, it may be easier to open the external file and make changes.
Editing Mechanical Desktop Parts Because interference was detected between the pulley plate and the DPULLEY3 parts, you need to enlarge the drilled holes on the pulley plate. Editing an external part updates all instances of the parts in the assembly drawing. The modified part retains the applied assembly constraints. In this tutorial, you return to the open ppulley.dwg file and make the holes larger, to remove the interference.
Reloading External References To update the assembly to reflect the changes you made to the external part, reload the external definition. To reload an external definition 1 Switch to the window containing the assembly. 2 Use AMCATALOG to reload the PPULLEY definition. Context Menu In the graphics area, right-click and choose Catalog. In the Assembly Catalog, in External Assembly Definitions, right-click PPULLEY and choose Reload. Choose OK. The pulley plate reflects the new design.
To check for interference 1 Use AMACTIVATE to activate the SUBPULLY subassembly. Context Menu In the graphics area, right-click and choose Assembly ➤ Activate Assembly. Specify the SUBPULLY subassembly. 2 Use AMINTERFERE to check for interference. Context Menu In the graphics area, right-click and choose Analysis ➤ Check Interference. 3 Specify DPULLEY3. No interference should be detected. Assigning Mass Properties Next, calculate mass property information.
3 In the Assembly Mass Properties dialog box Setup tab, specify: Output Units: Metric (mm, g) Coordinate System: User coordinate system (UCS) Display Precision: Select 0.00000 Part Name: Select BRACKET Materials Available: Material: Select Stainless_Steel Choose Assign Material. The material information is transferred to the part material attribute and BOM, and is updated in the part name list. Next, change the material definition for a part in the assembly.
To calculate mass properties 1 In the Mass Properties Dialog Box, select the Results tab. Then select the Calculate button. The results are calculated and displayed. The Calculate button is no longer available because the Setup and Results fields are in sync. If you change an item on the Setup tab, the results are cleared and the Calculate button becomes available. You can use the Insert UCS button to create and insert a user coordinate system (UCS) based on a parts or assemblies center of gravity (CG).
Reviewing Assembly Models Assembly scenes and drawing views are essential for reviewing the assembly model. For this lesson, you first create an exploded assembly scene, and then tweak the positions of parts and add assembly trails and annotations. Creating Exploded Assembly Scenes After assembly constraints have been applied to each part, you can create a scene (an exploded view of the entire assembly). Multiple scenes can be created and named.
The scene, design1, is displayed. 2 Look at the Browser. The names of all parts in the design1 scene are listed. Next, align the exploded parts in the assembly scene.
Using Tweaks and Trails in Scenes In an exploded scene, sometimes parts obscure other parts. You can use tweaks to change the positions of individual parts and then adjust the positions of the parts in the design1 scene. Zoom in to magnify the parts to be tweaked. In the Browser, tweaks are nested under the respective parts. You can select and multi-select tweaks in the Browser to delete them. When you pause the cursor over a tweak in the Browser, a tooltip displays the distance factor for the tweak.
In the Power Manipulator dialog box, on the Move tab, verify that Place Objects (ALT) is selected. Choose Done. NOTE To access the Power Manipulator dialog box later, right-click the Power Manipulator symbol on your screen, and select Options. 2 Use AMTWEAK to tweak the BUSHING part, responding to the prompts. Context Menu In the graphics area, right-click and choose New Tweak.
3 Continue on the command line. Select handle or Geometry [Undo/UCS/WCS/Select/Options/Pancenter/Type/tRails/X/Y/Z] : Press ENTER. 4 Use AMTWEAK to tweak the SHAFT part, responding to the prompts. Context Menu In the graphics area, right-click and choose New Tweak. Select part/subassembly to tweak: Specify a point on SHAFT_1 (1) Enter an option [Next/Accept] : Press ENTER The Power Manipulator symbol is displayed on the SHAFT part.
To adjust assembly trails 1 Use AMTRAIL to adjust your assembly trails, responding to the prompt. Command AMTRAIL The Trail Offsets dialog box is displayed. 2 Use the options in the Trail Offsets dialog box, to adjust over shoots and undershoots for your trails. Choose OK to apply your selections. Next, create an assembly drawing view. Creating Assembly Drawing Views An assembly drawing view shows a 2D representation of the 3D assembly. You use the base part for a base view.
To create a drawing view 1 Use AMDWGVIEW to create a new drawing view. Context Menu In the graphics area, right-click and choose New View. 2 In the Create Drawing View dialog box, specify: Type: Base Data Set: Scene: DESIGN1 Scale: Enter .03 (or .75 mm) Choose OK.
The base assembly drawing view is displayed. 4 Create an isometric view of the assembly. Context Menu In the graphics area, right-click and choose New View. In the Create Drawing View dialog box, specify: View Type: Iso Scale: Enter 1 Relative to Parent: Select the check box Choose OK.
6 Use AMMOVEVIEW to align the views, responding to the prompts. Context Menu In the graphics area, right-click and choose Move View. Select view to move: Select the isometric view Specify new view location or [Layout]: Align the views and press ENTER Examine the Browser. The isometric view is listed under the base view. Now, create a BOM database, and add a parts list and associative balloon callouts.
Creating Bills of Material After you have assembled your parts, you can create a bill of material (BOM) database. This database contains a list of attributes assigned to each part. The attributes store information such as manufacturer, description, and vendor part number. The attributes are contained in part references that are assigned to each part. Part references can also be created to reference other geometry in your drawing, such as surfaces. The geometry can then be included in a parts list.
Notice the SUBPULLY definition in the list of parts. The plus sign in front of it indicates that it is a subassembly. 2 Click the plus sign in front of SUBPULLY. The BOM database now lists all the parts in the assembly, including those in the subassembly. Choose OK to exit the BOM dialog box. 3 Select the Model tab in the browser. A BOM icon is located under PULLYASM. By default, the BOM takes the same name as the assembly file.
To modify symbol standards 1 Use AMOPTIONS to access the Mechanical Desktop symbol standards. Command AMOPTIONS In the Mechanical Options dialog box, expand the hierarchy of ANSI, and double-click the icon in front of BOM Support.
Choose Apply, then OK. The Mechanical Options dialog box is still open. 3 Choose OK to close the Symbol Standards dialog box. Save your file. Working with Part References When you create a BOM database, each part in the assembly is assigned a part reference. A part reference is an attributed block that can be modified to include any information you want to attach to the part. That information is used by the BOM database and included in the parts lists you generate.
To edit a part reference 1 Use AMPARTREFEDIT to edit a part reference, responding to the prompt. Context Menu In the graphics area, right-click and choose Annotate Menu ➤ Parts List ➤ Part Reference Edit. Select pick object: Select the part reference for BRACKET (1) 1 2 In the Part Ref Attributes dialog box, double-click in the Name field and enter Pulley Bracket. Choose OK.
3 Use AMBOM to display the BOM database. Context Menu In the graphics area, right-click and choose Parts List ➤ BOM Database. Bom table [Delete/Edit] : Press ENTER Notice that Pulley Bracket is now listed under Note for BRACKET. Choose OK to exit the BOM dialog box. Next, add balloon callouts to the isometric view. Adding Balloons Balloons are used to reference parts in your drawing to a parts list. They contain the same information as the part reference they are attached to.
To place a balloon callout 1 Use AMBALLOON to create balloon callouts for BRACKET, DPULLEY, BUSHING, SHAFT, and NUT3, responding to the prompts. Desktop Menu Choose Annotate ➤ Parts List ➤ Balloon.
Continue on the command line: Select pick object: Press ENTER Align Standalone/Horizontal/: Specify a point between the two drawing views Next, place the parts list in the drawing. Placing Parts Lists A parts list is an associative block of information about your assembly. It displays information about the parts, according to the settings specified in the BOM database.
To place a parts list 1 Use AMPARTLIST to place the parts list under the base view of your assembly, responding to the prompts. Context Menu In the graphics area, right-click and choose Parts List ➤ Part List. The Parts List dialog box is displayed. 2 In the Parts List dialog box, in Title, enter the new name Pulley Parts List. 3 Choose Apply, then choose OK. Specify location: Specify a point under the base view The parts list is placed in the drawing.
When the parts list is created, a parts list icon is displayed in the Browser. Save your file. Finishing Drawings for Plotting Now that the assembly has been documented, plot the drawing. Paper drawings are useful for reviewing the entire assembly to make sure that the design is feasible and can be manufactured. The Parts List on the assembly drawing provides information about the parts needed to manufacture the assembly.
532
Creating and Editing Surfaces In This Chapter This Autodesk® Mechanical Desktop®tutorial 19 ■ Creating surfaces—motion based, skin, and derived introduces surfaces grouped by function, and provides instructions for creating the different types of surfaces. ■ Joining and trimming surfaces ■ Editing surfaces You learn surface types, practice surface modeling, and work with modeling some typical surfaces.
Key Terms Term Definition augmented line A 3D polyline with vector information at each vertex. An augmented line is a surface creation tool that allows you to control the curvature and the tangency of a surface. base surface A basic underlying surface that carries a shape across a larger area. Can be trimmed to precise shapes as needed, but the base surface remains intact and may be displayed. derived surface A surface that gets some or all of its attributes from one or more base surfaces.
Basic Concepts of Creating Surfaces Three-dimensional surface modeling can be compared to constructing a building. You start by establishing the initial shape. Then you cover the rough framing with siding and roofing. rough frame siding applied One approach to surface modeling is to create a 3D framework of wires. Wire is a generic term for lines, arcs, circles, ellipses, 2D and 3D polylines, augmented lines, and splines, including splines created from existing part edges.
Working with Surfaces In this tutorial you’ll learn about these types of surfaces: ■ ■ ■ ■ Primitive, created by specifying values Motion-based, created by moving wires through space Skin, applied over a wireframe Derived, generated from existing surfaces Primitive surfaces (cone, cylinder, sphere, and torus) do not require wireframes for their construction. To create a sphere surface, for example, you determine the center of the sphere and then enter a value for its radius.
To set up your file 1 Open the file t_surfs.dwg in the desktop\tutorial folder. The wireframe objects you need for this lesson are included in this file. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40. Surface lines, called U and V lines, indicate the direction of the surface. Increasing the number of lines increases the density of the surface image.
Creating Motion-Based Surfaces Some surfaces are created by “moving” wires through space. These motionbased surfaces are revolved, extruded, and swept. Revolved Surfaces A revolved surface uses two wires: one establishes the constant shape of the surface, and the other is the axis about which to spin the shape. The revolved surface is created by the motion of a wire shape through space. To revolve a surface 1 Use AMREVOLVESF to revolve a spline curve about an axis, responding to the prompts.
Extruded Surfaces An extruded surface is created by a 3D wire shape moved along a straight line. You select a line, polyline, arc, or spline to extrude, and you specify the direction and magnitude of the extrusion. To extrude a surface 1 Use AMEXTRUDESF to extrude a circle into a cylinder, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Extrude Select wires to extrude: Select circle (1) Select wires to extrude: Press ENTER Define direction and length.
The extruded surface should look like this. 2 For more practice, choose Extrude again. Select the spline and then a location on the line to determine the length and direction. Because the line is obscured by the first surface you created, you may have difficulty selecting it. Press CTRL as you select, to cycle through the objects. Press ENTER when the line is highlighted. 3 Use the Zoom Extents option of ZOOM to redisplay all the wireframes and select the object for the next exercise.
To create a swept surface 1 Use AMSWEEPSF to sweep two cross sections along a rail, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: Select the first cross section (1) Select cross sections: Select the second cross section (2) and press ENTER Select rails: Select line (3) and press ENTER 2 3 1 2 In the Sweep Surface dialog box, choose OK to accept default settings. A message tells you that four surfaces will be created. Choose Continue.
You can select the individual surfaces to see the shape of each one. Because one of the cross sections has sharp corners, a single surface cannot be created. Instead, four separate surfaces are created, each corresponding to one side of the rectangular cross section. For more information, see “To surface polylines with sharp corners” on page 550. 3 Use the Extents option of ZOOM to redisplay all the wireframes and select the object for the next exercise.
You created a nonuniform rational B-spline (NURBS) surface from a spline. You can convert a NURBS surface into a part by adding thickness. NOTE Save a copy of your NURBS surface if you will need it later. When you thicken a surface, the original surface is consumed and disappears. To convert a NURBS surface to a solid 1 Use AMTHICKEN to convert a NURBS surface to a thin solid, responding to the prompts.
To sweep dissimilar shapes 1 Sweep two dissimilar shapes along two nonparallel rails, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: Select first shape (1) Select cross sections: Select second shape (2) and press ENTER Select rails: Select first rail (3) Select rails: Select second rail (4) 1 3 4 2 2 In the Sweep Surface dialog box, choose OK to accept the default settings. The swept surface should look like this.
To sweep multiple cross sections along two rails 1 Sweep multiple cross sections along two rails, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: Select cross sections (1) through (5) in consecutive order and press ENTER Select rails: Select first rail (6) Select rails: Select second rail (7) 1 2 6 7 3 4 5 2 In the Sweep Surface dialog box, choose OK to accept the default scale. Because the cross sections have rounded corners, a single surface results.
Creating Skin Surfaces A skin surface drapes over a wireframe model. After the wireframe is removed, the surface retains the shape of the wireframe. Skin surfaces are ruled, planar, lofted U, and lofted UV. Ruled Surfaces A ruled surface is a straight, flat shape stretched between two wires of any 3D shape. You can create a ruled surface between any two nonintersecting wires that can represent the top and the bottom. The top and bottom can be open or closed wires.
The ruled surface shows the surface normal, a short vertical line in one corner. A surface normal shows where the surface starts and which direction is out. If surface normal indicators are too small, use the DISPSF system variable to change the size. In the Individual Surface Display dialog box, change the value in the Normal Length field. Adjust the setting as needed. You can create a ruled surface from two augment lines, or by adding width to a single augmented line.
To surface an augmented line 1 Use AMRULE to create a surface from the augmented wire, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Rule Select first wire: Select the augmented line Enter an option [Next/Accept] : Press ENTER Enter width (or) [Select second wire] <1.0000>: Press ENTER The surface extends beyond the vectors to the specified width. You can use this technique to create a ruled surface normal to any existing ruled surface.
To surface two arcs with different radii 1 Create a surface from two arcs of different radii, responding to the prompts. Surface ➤ Create Surface ➤ Rule Desktop Menu Select first wire: Select arc (1) Select second wire: Select arc (2) 1 2 The ruled surface should look like this. surface normal 2 To experiment, use the previous example and select the arcs in a different order. 3 Erase the surface you just created. Desktop Menu Modify ➤ Erase Select the surface and press ENTER.
Selecting the arcs in different order changes the surface normal. surface normal 5 Use the Extents option of ZOOM to redisplay all of the wireframes and select the object for the next exercise. In the next exercise, you surface polylines. A surface follows a spline exactly but approximates the polyline by a curve. The Polyline Fit default setting of 150 maintains all corners less than 150 degrees as sharp corners. In such cases, multiple surfaces are created.
Choose OK. These settings force sharp corners to convert to a smooth curved surface. 3 Choose OK to exit the Mechanical Options dialog box.
4 Use AMRULE to create a curved surface from polylines drawn with sharp corners, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Rule Select first wire: Select polyline (1) Select second wire: Select polyline (2) 1 2 A continuous smooth curved surface is created. 5 Use the Extents option of ZOOM to redisplay all of the wireframes and select the object for the next exercise. Now use the same polylines, but choose a fit angle to recognize sharp corners.
To create surfaces with sharp angles 1 Use AMOPTIONS to reset the fit angle to 150 and re-create the ruled surface. Desktop Menu Surface ➤ Surface Options 2 Erase the surface you just created. Desktop Menu Modify ➤ Erase 3 Use AMRULE to create three ruled surfaces from polylines drawn with sharp corners, responding to the prompts.
5 Use the Extents option of ZOOM to redisplay all of the wireframes and select the object for the next exercise. Trimmed Planar Surfaces A planar surface may be constructed from lines, arcs, splines, polylines, or simply two locations, if the selected objects are closed and on the same plane. The exterior shape of the 2D wire shape becomes the trimmed edge of the surface. In this exercise, you create trimmed planar surfaces.
To create a trimmed planar surface using three closed polylines 1 Create a planar trim surface from three polylines, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Planar Trim Specify first corner or [Plane/Wires]: _wire Select wires: Select object (1) Select wires: Select interior circle (2) Select wires: Select circle (3) Select wires: Press ENTER 1 2 3 Instead of selecting the objects individually, you could also drag a crossing window around all of them and press ENTER.
A lofted U surface is stretched between any number of wires that share similar characteristics. The example contains two sets of wires from which you create two surfaces. The light blue polylines are approximately horizontal, and the green lines are approximately vertical. First, you create a surface from the horizontal polylines. To create a lofted surface using a set of wires 1 Use AMLOFTU to surface a set of vertical wires, responding to the prompts.
3 Surface a set of horizontal wires, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ LoftU Select U wires: Select lines (9) through (18) in consecutive order and press ENTER 4 In the Loft Surface dialog box, choose OK to accept the default settings. The two surfaces, one horizontal and one vertical, should look like these. 5 Use the Extents option of ZOOM to redisplay all the wireframes and select the object for the next exercise.
To create a single lofted surface from two groups of wires 1 Group the magenta U lines. Command GROUP In the Object Grouping dialog box specify: Group Name: Enter uwires Create Group: Choose New to close the dialog box Respond to the prompt as follows: Select objects: Select lines (1) through (7) in consecutive order and press ENTER In the Object Grouping dialog box, choose OK. 2 Press ENTER to repeat the GROUP command.
3 Use AMLOFTU to loft a surface from two groups of wires, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ LoftUV Select U wires: Enter g Enter group name: Enter uwires 7 found Select U wires: Press ENTER Select V wires: Enter g Enter group name: Enter vwires 6 found Select V wires: Press ENTER Enter an option [eXit/Loft/Node check] : Press ENTER You have created a surface from the two groups of wires.
To create a blended surface 1 Use AMBLEND to create a blended surface from two wires, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Blend Select first wire: Select surface (1) Select second wire: Select surface (2) Select third wire [Weights]: Press ENTER 1 2 You have created the first blended surface. The type of object you select affects the blended surface. When you select surfaces or augmented lines, you are prompted for the weight of the surface edge.
3 Create the third blended surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Blend Select first wire: Select surface (5) Select second wire: Select surface (6) Select third wire [Weights]: Press ENTER 5 6 4 Use ZOOM to enlarge the corner area created by the blended surfaces. 5 Use AMBLEND to create a corner blended surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Blend.
Use the Extents option of ZOOM to redisplay all of the wireframes and select the object for the next exercise. Next, you create a blended surface from two surfaces and lines. To create a blended surface from four objects, make the selections in the order shown; the objects cannot be selected in consecutive order. To blend surfaces and lines 1 Use AMBLEND to create a surface from two surfaces and two lines, responding to the prompts.
To blend augmented lines 1 Use AMBLEND to create a surface from two augmented lines, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Blend Select first wire: Select line (1) Select second wire: Select line (2) Select third wire [Weights]: Press ENTER 2 1 2 Use ZOOM to redisplay wireframes. Then select the second set of lines. 3 Create a surface from the second set of augmented lines, responding to the prompts.
To create an offset surface 1 Use AMOFFSETSF to create an offset surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Offset Select surfaces to offset: Select surface (1) Select surfaces to offset: Press ENTER Distance=1.0000 Keep=Yes Enter offset distance or [Keep] <1.0000>: Enter k Keep original surface(s) [Yes/No] : Enter y Distance=1.0000 Keep=Yes Enter offset distance or [Keep] <1.0000>: Enter 0.
Fillet and Corner Surfaces In this exercise, you create fillet surfaces between two selected surfaces, and a corner fillet where three fillet surfaces intersect. You trim the original surfaces back to the fillet surfaces. To create fillet and corner surfaces 1 Use AMFILLETSF to create a fillet between two surfaces, responding to the prompts.
3 Create a fillet between another two surfaces, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Fillet Select first surface or quilt interior edge: Select surface (3) Select second surface: Select surface (4) 3 4 4 In the Fillet Surface dialog box, specify: Fillet Type: Constant Trim: Both Surfaces Create To: Base Surface Radius: Enter 0.75 Choose OK. The Base Surface option was not available when you created the first fillet surface.
The next illustration shows both fillets, which you will trim later. 5 Create a fillet between another two surfaces, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Fillet Select first surface or quilt interior edge: Select surface (5) Select second surface: Select surface (6) 6 5 6 In the Fillet Surface dialog box, specify: Fillet Type: Constant Trim: Both Surfaces Create To: Base Surface Radius: Enter 0.6 Choose OK. The fillets overlap at the corner.
To create a corner fillet 1 Use AMCORNER to trim the overlapping fillets, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Corner Fillet NOTE The default is set to trim the corner fillet to the three fillet surfaces. If you do not want to trim, enter T at the first prompt and change the setting to No.
Editing Surfaces As you create models, you need to combine surfaces and trim them where they overlap. You will learn four surface editing techniques: adjusting surfaces, joining surfaces, trimming surfaces at intersections, and trimming surfaces by projection. Adjusting Adjacent Surfaces You can control the tangency of two adjacent surfaces by adjusting them to create one continuous surface. When you select the edges of two adjacent surfaces to adjust, the first edge you select is the control surface.
First surface=20.0000% Second surface=20.0000% cOntinuity=Smooth Keep=No Enter an option [First surface/Second surface/cOntinuity/Keep] : Enter s Enter adjustment for the second surface <20.0000%>: Enter 40 First surface=20.0000% Second surface=40.0000% cOntinuity=Smooth Keep=No Enter an option [First surface/Second surface/cOntinuity/Keep] : Enter o Continuity [Coincident/Smooth] : Press ENTER First surface=20.0000% Second surface=40.
1 2 The two surfaces are joined. Only one surface normal indicator is shown. To force two surfaces to join, choose Surface ➤ Surface Options. In the Mechanical Options dialog box, choose the Surface tab and adjust the Join Gap Tolerance. Two untrimmed surfaces are joined automatically if they are within twice the gap tolerance. 2 Use the Extents option of ZOOM to redisplay all of the wireframes and select the object for the next exercise.
To trim intersecting surfaces 1 Use AMINTERSF to trim the surface you want to keep, responding to the prompts. Desktop Menu Surface ➤ Edit Surface ➤ Intersect Trim Select first surface/quilt or wire: Select surface (1) Select second surface: Select surface (2) 2 1 2 In the Surface Intersection dialog box, check the options indicated in the following illustration and choose OK. The first surface you selected is trimmed at its intersection with the second surface.
1 3 Use UNDO to erase the trim. Then try selecting surfaces at different locations. 4 Use the Extents option of ZOOM to redisplay all of the wireframes and select the object for the next exercise. Trimming Surfaces by Projection You can project a wire onto a surface to trim a shape that corresponds to the wire shape. You select the portion of the surface you want to keep. In this exercise, you trim a curved surface with a star-shaped polyline.
2 In the Project to Surface dialog box, specify: Direction: Choose Normal Output Type: Choose Trim Surface Keep Original Wire: Check the check box Choose OK. The polyline is projected onto the curved surface, trimming out the surface inside the polyline. 3 Use UNDO and try different selection points and output types for the projection.
Combining Parts and Surfaces In This Chapter In Autodesk® Mechanical Desktop®, surfaces are 20 ■ Creating a part with multiple features valuable features because they can represent complex curved shapes. When joined to a parametric part, they ■ Creating a simple surface ■ Attaching a surface parametrically to a part cut away an angular surface and replace it with a sculpted face. A surface may also add material to a part as a protrusion.
Key Terms Term Definition base surface A basic underlying surface that carries a shape across a larger area. Can be trimmed to precise shapes as needed, but the base surface remains intact and may be displayed. model view Changes orientation of the viewer so that the object is viewed from a different position. Individual views can be displayed in multiple viewports. For example, enter 3 at the Command prompt to create three viewports with default views: top, front, and right isometric.
Basic Concepts of Combining Parts and Surfaces You can use Mechanical Desktop® to create angular-shaped parts. You can apply 3D surfaces to those parts to create hybrid parts consisting of a mixture of angular and curved shapes. With Mechanical Desktop you can create model designs with shapes of varying types. You can apply surfaces to Mechanical Desktop parts and use those surfaces to cut material from a parametric part, to create any hybrid shapes that your design requires.
First, sketch the camera from all sides (top, side, front, and isometric views). With a complete idea, you can decide where to place features on the camera body. shutter release mount film advance mount lens sheath viewfinder compartment flash compartment film compartment battery compartment door cutout The camera body, which is common to all other features, is the base feature.
Creating Surface Features Open the file camera.dwg in the desktop\tutorial folder. The file contains the settings you need, and the geometry to create the camera body—an extruded feature and some NURBS curves. You use NURBS to create the surface for the sculpted camera face. NOTE Back up the tutorial drawing files so you still have the original files if you make a mistake. See “Backing up Tutorial Drawing Files” on page 40.
To create a swept surface 1 Use AMSWEEPSF to sweep a spline along a rail, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: In the front view, choose the right horizontal spline (1) Select cross sections: Press ENTER Select rails: Select the vertical spline (2) Select rails: Press ENTER 2 3 1 2 In the Sweep Surface dialog box, specify: Orientation: Parallel Choose OK. The first half of the swept surface is created.
4 Use AMJOINSF to join the two surfaces, responding to the prompts. Desktop Menu Surface ➤ Edit Surface ➤ Join Select surfaces to join: Select the right surface (1) Select surfaces to join: Select the left surface (2) and press ENTER 2 1 The two surfaces create a single surface. The resulting surface probably does not extend beyond the part on all sides, so you need to lengthen the surface. 5 Use AMLENGTHEN to lengthen the surface, responding to the prompts.
Attaching Surfaces Parametrically Next, you create a work plane and work point and then dimension the work point to the part. This dimension establishes a parametric relationship between the surface and the part. The position of the surface is controlled by the work point, and its orientation is controlled by the work plane associated with the work point. Later, if you modify the position of the work point, the surface location moves accordingly.
1 2 You have created a parallel work plane offset from the front face of the part. 3 Use AMWORKPT to place a work point on the work plane, responding to the prompts. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Work Point. Workpoint will be placed on the current sketch plane. Specify the location of the workpoint: Specify a location (2) You have created a work point on the sketch plane.
5 Continue on the command line. Select first object: Select the work point Select second object or place dimension: Select the bottom edge of the camera body Specify dimension placement: Place the vertical dimension Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.8898>: Enter 1 Solved fully constrained sketch. Select first object: Press ENTER The work point is fully constrained. Save your file.
One side of the part is cut away, leaving the curved face of the surface. Your model shows the modified block and the splines used to create the surface. 2 Use REGENALL to regenerate the drawing views. Desktop Menu View ➤ Regen All 3 Remove the three splines used to create the surface. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Erase. 4 Select the three splines and press ENTER. Save your file.
Creating Extruded Features The film compartment at the back of the base feature has two features—the compartment and the door. The camera back is a flat plane. You specify it as the sketch plane, sketch the profile, and extrude it directly into the camera body. To sketch the film compartment 1 Use AMSKPLN to create a new sketch plane, responding to the prompts. Work in the isometric view. Context Menu In the graphics area, right-click and choose New Sketch Plane.
3 Use RECTANG to sketch a rectangle to the left on the camera back. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Rectangle. 4 Use AMPROFILE to create a profile from the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. You need to place four dimensions or constraints: two to define the sketch size and two to specify the sketch location on the camera body.
3 Make the isometric view active. To see the dimensions and the profile sketch more clearly, rotate the isometric view until the back of the camera faces you. Desktop Menu View ➤ 3D Views ➤ Back Left Isometric Define the distance between the top of the sketch and the top of the camera back. 4 Use AMPARDIM to constrain the rectangle to the camera body, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension.
To cut the film compartment 1 Use AMEXTRUDE to cut the film compartment from the camera body. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Operation: Cut Termination: Blind Distance: Enter 1.2 Flip: Point the direction arrow into the camera body Choose OK. The cut-out compartment is displayed in all four views.
2 Activate and then restore the viewports to the original orientation. Upper right viewport: Front Right Isometric View Lower left viewport: Front View Cutting the door is similar to cutting the film compartment. You sketch a rectangle on the right side of the camera and blindly extrude it as a cut into the camera body. To sketch the film compartment door 1 Use AMSKPLN to create a new sketch plane, responding to the prompts. Work in the isometric view.
2 Set the UCS origin to the lower-left corner of the right side of the camera, responding to the prompts. Desktop Menu Assist ➤ New UCS ➤ Origin Specify new origin point <0,0,0>: Enter end of: Specify a point near the lower-left corner of the side view NOTE If the UCS icon does not snap to the lower-left corner of the camera, set the AutoCAD system variable UCSICON to On. 3 In the side view, zoom in on the camera face. Context Menu In the graphics area, right-click and choose Zoom.
To constrain the film compartment door 1 Use AMADDCON to make the bottom edge of the profile sketch collinear with the bottom line of the film compartment, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Constraints ➤ Collinear.
3 Use AMPARDIM to dimension the width and height of the profile sketch, responding to the prompts. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. Select first object: Select a horizontal profile edge Select second object or place dimension: Place the horizontal dimension Enter dimension value or [Undo/Hor/Ver/Align/Par/aNgle/Ord/Diameter/pLace] <0.6840>: Enter .6 Solved underconstrained sketch requiring 1 dimensions or constraints.
2 Choose OK to create the extrusion. Save your file. The battery compartment also has a cutout for a door. The order in which you create these features does not matter, but the natural order would be to create the film compartment first. The cutout for the battery compartment is more complicated because of its shape. The key to creating this feature is to locate the sketch plane properly on the bottom left side of the camera body.
3 Use PLINE to sketch the profile of the battery compartment on the bottom of the camera body. Work in the bottom view. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Polyline. 4 Use AMPROFILE to create the profile sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. The sketch needs seven to nine dimensions or constraints, depending on how precisely you drew the sketch.
3 Use AMPARDIM to add the following dimensions. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. The sketch is fully constrained. To cut the battery compartment 1 Use AMEXTRUDE to cut the profile from the camera body. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Operation: Cut Termination: Blind Distance: Enter 2.4 Flip: Point the direction arrow into the camera body Choose OK.
To sketch and constrain the battery compartment door 1 Use RECTANG to sketch the profile of the cutout. Work in the bottom view. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Rectangle. 2 Use AMPROFILE to create the profile sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. The sketch requires four dimensions or constraints. 3 Use AMADDCON to constrain the sketch to the bottom of the camera body.
To cut the battery compartment door 1 Use Extrude to cut the door opening from the camera body. Make sure the direction of the cut is into the camera body. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Operation: Cut Termination: Blind Distance: Enter .1574 Flip: Point the direction arrow into the camera body Choose OK. Save your file.
In the Hole dialog box, select the Counterbore hole type icon and specify: Termination: Blind Placement: 2 Edges Dia: Enter .5 Depth: 1.0 Pt. Angle: Enter 180 C’Dia: Enter .65 C’Depth: Enter 1 Choose OK. 4 Respond to the prompts as follows: Select the first edge: Select the top, back edge in the isometric view (1) Select the second edge: Select the top, left edge in the isometric view (2) Specify the hole location: Specify a location (3) Enter the distance from first edge (highlighted) <0.4146>: Enter .
A hole is created for the film advance component. 5 Press ENTER to redisplay the Hole Feature dialog box. Specify: Operation: C’Bore Termination: Blind Placement 2 Edges Drill Size: Custom, enter .2 diameter, 1.0 depth, and 180 degrees point angle C’bore/Sunk Size: Enter .3 diameter and .
Creating Features on a Work Plane The camera body is complete except for features on the camera face. Unlike the previous features, you sketch these features on a work plane parallel to the front of the camera. You extrude the features from the work plane and into the camera body to the correct depth. You sketch on the work plane because 2D sketches cannot be drawn and profiled on a NURBS surface.
2 Respond to the prompts as follows: Select work plane, planar face or [worldXy/worldYz/worldZx/Ucs]: Specify a point (1) Enter an option [Next/Accept] : Press ENTER when the front of the camera is selected Enter an option [Flip/Accept] : Verify that the work plane is offset from the camera front and press ENTER Plane = Parametric Select edge to align X axis or [Flip/Rotate/Origin] : Point the Z axis away from the camera front and press ENTER 1 The work plane is created in front of
To position the circle, you need three dimensions or constraints: a diameter and two dimensions to locate the circle on the sketch plane relative to the camera body. 5 Use AMPARDIM to dimension the sketch with the following values. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. 6 Use EXTRUDE to extrude the profile to create the outer cover of the lens sheath. Work in the isometric view.
To hollow out the lens sheath 1 Activate the front view, and sketch a circle on the work plane. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Circle. 2 Profile the sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. Three dimensions or constraints are needed to solve the sketch. 3 Use AMADDCON to constrain the sketch to be concentric with the lens sheath, responding to the prompts.
In the Extrusion dialog box, specify: Operation: Cut Termination: Through Flip: Point the direction arrow into the camera body Choose OK. Save your file. Next, you create the viewfinder compartment, a filleted rectangle that is cut from the camera face. To cut the viewfinder compartment 1 Use RECTANG to sketch a rectangle on the sketch plane above the lens sheath. Work in the isometric view. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Rectangle.
4 Use AMPROFILE to create the profile sketch. Context Menu In the graphics area, right-click and choose Sketch Solving ➤ Single Profile. You need five or more dimensions or constraints to solve the sketch. Add the dimensions for the length and width of the shape, one dimension for the fillets, and two dimensions to locate the sketch in relationship to the camera body. 5 In the front view, zoom in to enlarge the model as needed. 6 Use AMPARDIM to add the following dimensions.
To cut the flash compartment 1 Sketch a rectangle to the right of the viewfinder. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Rectangle. 2 Define a fillet for the corners of the rectangle, responding to the prompts. Context Menu In the graphics area, right-click and choose 2D Sketching ➤ Fillet. Current settings: Mode = TRIM, Radius = 0.5000 Select first object or [Polyline/Radius/Trim]: Enter r Specify fillet radius <0.5000>: Enter .1 3 Press ENTER to restart FILLET.
6 Add the following dimensions. Context Menu In the graphics area, right-click and choose Dimensioning ➤ New Dimension. 7 Extrude the sketch to cut it through the camera body. Context Menu In the graphics area, right-click and choose Sketched & Work Features ➤ Extrude. In the Extrusion dialog box, specify: Operation: Cut Termination: Through Flip: Point the direction arrow into the camera body Choose OK. Save your file.
Modifying Designs As with all projects, designs change during the development process. For example, you might want to scale the camera to a smaller size and change the dimension that positions the camera face on the solid model. Because you want both the surface and the camera body at the same scale, you first resize them. In this exercise, you specify a percentage of the camera’s current size. Then, to position the surface on the camera proportionately, you modify the parametric dimension.
To reposition the camera face 1 Use AMEDITFEAT to edit the surfcut feature, responding to the prompts. Context Menu In the graphics area, right-click and choose Edit Features ➤ Edit. Enter an option [Sketch/surfCut/Toolbody/select Feature]
Finishing Touches on Models The finishing touch for the camera body is to fillet the corners where the different sides meet. To finish the camera body 1 Use AMVISIBLE to hide the work plane from your display. Desktop Menu Part ➤ Part Visibility 2 In the Desktop Visibility dialog box, select the Part tab and choose Work Planes and Hide. Choose OK. 3 Use ISOLINES to increase the number of isolines. Change the value to 8 to show more detail on the model. The display will change when you edit your model.
6 Fillet the outside corners and edges of the camera body. When you are finished, choose Done. The camera body is finished.
Surfacing Wireframe Models In This Chapter This Autodesk® Mechanical Desktop® tutorial introduces 21 ■ Studying the design intent and developing a strategy wireframe surface modeling, one of the key uses for surface modeling. You learn how to develop a strategy for a surfacing project, and how to achieve the design intent.
Key Terms Term Definition base surface A basic underlying surface that carries a shape across a larger area. Can be trimmed to precise shapes as needed, but the base surface remains intact and may be displayed. logical surface area An area that can be described by a single surface. projected wire A 2D line that represents an opening on a surface and trims a hole in the surface. Can also be a 3D polyline that represents the extents of the opening in the wireframe.
Basic Concepts of Surfacing Wireframe Models A completely surfaced model is a single electronic master suitable for engineering and manufacturing activities, such as: ■ ■ ■ ■ ■ ■ Generating accurate sections for engineering and packaging studies. Providing input for finite element modeling and analysis. Producing shaded renderings for marketing. Providing input for rapid prototyping equipment. Supplying rotated surfaces for tool, mold, and die design.
Review the wireframe in detail, to determine where you will have design challenges. Consider the following: ■ ■ ■ ■ The complexity of the surfaces you need to create. For example, what curvature is required of surfaces? Is it sufficient to have surfaces with no curvature (such as ruled surfaces), or do you need surfaces with multiple curvatures? How you can simplify shapes. Surfaces created from polylines or splines with a large number of points are complex and greatly increase computation time.
Likewise, the side of the top part of the pump constitutes a single surface. Each of these two surface areas requires a surface because no single surface could cover both. Surfaces can contain multiple wires. wireframe surface All lines inside the four boundaries share the same smooth curvature as the boundary edges. There are no abrupt curvature changes, so the goal is to surface the entire area with a single surface, using the additional wires to constrain the surface shape.
In general, use only smooth wires to create surfaces. When you use a wire with sharp corners, those sharp areas do not produce an acceptable surface. wireframe unacceptable surface You need to find some other way to surface the area. Consider the design intent again. A second look at the area reveals a flat surface on the front of the pump housing that intersects a smoothly curved surface at the bottom.
A surface like this one is a basic surface that carries a shape across larger areas. This surface is referred to as a base surface. Even after many areas of the surface are trimmed away, the underlying base surface remains intact and may be displayed at any time with the Surface Display dialog box. base surface trimmed surface Identifying base surfaces is an important part of wireframe surfacing. Another approach is to categorize surfaces by type and eliminate those you won’t need.
If you are in doubt about whether a given area is flat, try to make a planar surface. A planar surface requires a single closed wire as its boundary. wire planar surface If the wire is not a closed single loop, you can see the breaks in the wire when you select it. closed wire multiple wires You can join line segments into a closed wire that forms the boundary of a planar surface. The surface is trimmed to the boundary shape.
In this example, the top area of the pump is not suitable for a single surface because there are abrupt changes in its smoothness. The center area is curved in one direction but straight in the other. When you have a surface area that can be defined by a straight line between two curves, you can create a ruled surface between the two curves. possible surface wire Look beyond the obvious visible surface to find a workable solution.
You can see that each end of the area beneath the inlet is described by lines with curvatures in both directions. This offers you a choice of surfacing methods, such as a swept surface or a lofted UV surface. swept surface lofted UV surface In most cases, there is more than one way to surface an area. Try both methods here, compare the results, and choose the one that produces the best result. ■ ■ Swept surfaces give you more control over the shape of the mid portion of the surface.
The easiest method is to use a single rail and a single section to surface the entire area, then trim the base surface to the intersecting part of the pump. section rail surface trimmed surface This choice might not always be correct. As you gain experience, you can predict which approach yields the most accurate results. In the previous example, verify that the surface created without the top line matches the top line within a reasonable tolerance.
Surfacing Wireframe Models Now that you have analyzed approaches to surfacing the pump housing and practiced surfacing techniques, you are ready to surface the pump. A surface modeling project may begin with a wireframe, whether it is a DXF or an IGES file from a client, or a 2D or 3D CAD design you created yourself. In order to describe the 3D object, most designers begin with a 2D drawing. In this lesson, you create surfaces for an actual part, a wireframe model of a hydraulic pump.
Notice that the values have changed in the Mechanical Options dialog box. These settings affect the visual representation of the surfaces and the size of the surface normal. Choose OK to exit. NOTE If you shade the surfaces you create to better view them, adjust the AutoCAD® setting that controls back faces. Go to Assist ➤ Options and select the System tab. Choose Properties and clear the check box beside Discard back faces. Choose Apply & Close, then OK.
Creating Trimmed Planar Surfaces Begin by surfacing the top section of the pump model, creating the individual surfaces. Top A is a planar surface because it is flat with sharp edges. Tops B and C are swept surfaces, bounded by curved wires. Top B uses two curves and two rails, and top C uses one curve and one rail. You trim the top C surface where it extends beyond the wireframe boundary. As you gain experience using the menu selections that correspond to commands, you may want to use shortcuts.
Select wires: Select wire (1) and press ENTER 1 6 2 4 7 3 5 A planar surface, trimmed to the boundary of wire (1), is created on the top of the model. To sweep a surface on two wires and two rails 1 Use AMSWEEPSF to create the top B surface, responding to the prompts.
To sweep a surface on one wire and one rail 1 Use AMSWEEPSF to create the top C surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: Select wire (6) and press ENTER Select rails: Select wire (7) and press ENTER In the Sweep Surface dialog box, in Orientation select Normal. Choose OK. The surface extends beyond the far side of the top. You will trim it later. 2 Move surfaces A, B, and C to the TOP layer, responding to the prompts.
To create a ruled surface between wires 1 Use AMRULE to create the top D surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Rule Select first wire: Select wire (1) Select second wire: Select wire (2) 3 4 5 2 1 2 Use BREAK to separate line segment (4) from polyline (3), responding to the prompts.
Next, break and join lines that are needed to create the top F planar surface. trimmed planar surface To create a planar surface with a joined polyline boundary 1 Use BREAK to break polyline (1) where it intersects polyline (2), responding to the prompts.
3 In the Join3D dialog box, specify: Mode: Automatic Output: Polyline Gap Tolerance: Enter .004 Choose OK. 4 Respond to the prompts as follows: Select start wire or: Select polyline (1) Select wires to join: Select polylines (2) through (5) Select wires to join: Press ENTER Reverse direction? [Yes/No] : Press ENTER to accept the direction of the new wire 5 1 2 4 3 To confirm that the segments are joined, select the polyline and check the grip points.
5 Use AMPLANE to create the top F surface from the joined polyline, responding to the prompt. Desktop Menu Surface ➤ Create Surface ➤ Planar Trim If you use the command line method, enter w at the prompt before continuing to the following prompt. Select wires: Select the joined polyline and press ENTER You have created the trimmed planar surface. Save the file. For the top G surface, extrude a polyline along a straight line, and then trim the surface to the desired shape.
Your selection point determines the extrusion direction. Select a point on polyline (2) close to polyline (1). If you select a point beyond the midpoint of polyline (2), the direction of the extrusion is reversed. Your drawing should look like this. 3 Move top F and top G to the TOP layer, responding to the prompts.
6 In the Surface Intersection dialog box, specify: Type: Trim Trim: Select both First Surface and Second Surface Clear the checkbox for Output Polyline Choose OK. The surfaces are trimmed where they intersect. Save the file. Joining Surfaces on Complex Shapes Next, you surface the inlet portion of the pump. Because the inlet has a complex shape, you will need five surfaces to represent its shape. ■ ■ ■ ■ 634 | Inlets A and C are ruled surfaces because they follow two polylines.
inlet A inlet E inlet B inlet D inlet C NOTE Be sure to select surfaces and lines where indicated on the illustrations. To select precisely, zoom in as needed. To create the inlet A ruled surface 1 From the Desktop menu, choose Assist ➤ Format ➤ Layer. In the Layer Properties Manager dialog box, thaw layer 20 and make it current. Then freeze layer 10 and TOP. 2 Change to a right isometric view.
4 Move the inlet A surface to the INLET layer, responding to the prompts. Command CHPROP Select objects: Select inlet A surface and press ENTER Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]: Enter La Enter new layer name <20>: Enter inlet Enter property to change [Color/LAyer/LType/ltScale/LWeight/Thickness]: Press ENTER Inlet B is an extruded partial cylinder, trimmed to its final shape by a closed wire. The surface is extruded across the inlet wireframe.
A close look at the inlet reveals that the extruded surface extends beyond the wireframe. You trim the inlet B surface to the boundary of surface D. 2 Use AMPROJECT to project the edge of inlet D to trim the inlet A surface, responding to the prompts.
To create the inlet C ruled surface 1 Use AMRULE to create the inlet C surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Rule Select first wire: Select wire (1) Select second wire: Select wire (2) 1 2 Your model should look like this. 2 Use CHPROP to move inlet B and C surfaces to the INLET layer. Save the file. Next, you create inlet D, a surface blended from the edges of inlet B and C surfaces and the polyline that defines the edge of inlet E.
To create the inlet D blended surface 1 Use BREAK to break the polyline into two line segments, responding to the prompts. Desktop Menu Modify ➤ Break Select object: Select polyline (1) Specify second break point or [First point]: Enter f Specify first break point: Enter int of: Select polyline (2) Specify second break point: Enter @ 1 2 Check the grip points of the line segments after you break the polyline. 2 Use AMBLEND to create the inlet D surface, responding to the prompts.
The blended surface should look like this. 3 Use CHPROP to move the surface to the INLET layer. Join the lines to form the boundary of inlet E, and then create a trimmed planar surface from the joined lines. Zoom in as needed to make line selection easier. To create the inlet E trimmed planar surface 1 Use AMJOIN3D to join selected lines to form the boundary for the inlet E surface.
This procedure joins lines regardless of their original direction and converts arcs and splines into polylines. You may need to reset the gap tolerance to correctly join the polylines. 3 Use AMPLANE to create a trimmed planar surface from the joined lines, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Planar Trim If you choose the command line method, enter w at the prompt before continuing to the following prompts.
To create a shape on a surface using joined wires 1 Thaw layers 10 and 20. 2 Change to the front right isometric view. Desktop Menu View ➤ 3D Views ➤ Front Right Isometric 3 Use BREAK to break the polyline, responding to the prompts.
1 2 5 Use AMJOIN3D to combine three polyline segments. Desktop Menu Surface ➤ Edit Wireframe ➤ Join In the Join3D dialog box, specify: Mode: Automatic Output: Polyline Gap Tolerance: Enter .004 Choose OK. 6 Respond to the prompts as follows: Select start wire or: Select polyline (1) Select wires to join: Select wire (2) Select wires to join: Select wire (3) and press ENTER Reverse direction? [Yes/No] : Press ENTER 1 2 3 The segments are joined together.
To trim a surface using a projected wire shape 1 Freeze layer 10 and thaw the TOP layer. 2 Return to the front right isometric view. Desktop Menu View ➤ 3D Views ➤ Front Right Isometric 3 Use AMPROJECT to cut top B where the inlet fits, responding to the prompts.
Creating Swept and Projected Surfaces For the main body of the pump, you continue building and trimming surfaces to their correct shapes. ■ ■ Body A, B, and C are swept surfaces created from curves and rails. Body D is a surface created from the boundaries of Body A, B, and C surfaces. body B body A body D body C To create the body A, B, and C swept surfaces 1 Thaw layer 30 and make it current. Freeze layers 10, 20, and TOP. 2 Use AMSWEEPSF to create the body A surface on the right side of the model.
Respond to the prompts: Select cross sections: Select wire (1) Select cross sections: Select wire (2) and press ENTER Select rails: Select wire (3) Select rails: Select wire (4) 5 1 6 3 4 2 7 8 3 In the Sweep Surface dialog box, specify: Transition: Scale Keep Original Wires: Check the check box Choose OK 4 Use AMSWEEPSF to create the body B surface on the left side of the model, responding to the prompts.
5 In the Sweep Surface dialog box, under Orientation, specify Normal. Leave Keep Original Wires checked, and choose OK. 6 Create the body C surface near the bottom of the model, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: Select wire (7) and press ENTER Select rails: Select the wire (8) and press ENTER 7 In the Sweep Surface dialog box, under Orientation, specify Normal. Verify that Keep Original Wires is checked, and choose OK.
To trim a surface with a projection wire 1 Use AMPROJECT to trim the body surface with the inlet edge, responding to the prompts. Desktop Menu Surface ➤ Edit Surface ➤ Project Trim Select wires to project: Select wire (1) Select wires to project: Press ENTER Select target surfaces/quilts: Select surface (2) Select target surfaces/quilts: Press ENTER 1 2 2 In the Project to Surface dialog box, specify: Direction: Normal Output Type: Trim Surface Verify that Keep Original Wires is checked, and choose OK.
body surface removed 3 Freeze layer 20. Cut out the surface areas on body C where body D and the outlet (to be surfaced later) extend onto body C.
To trim the body C surface with projection wires 1 Change to the front view of your model. Desktop Menu View ➤ 3D Views ➤ Front 2 Trim Body C with the lower curve of the flat surface (1), responding to the prompts.
Your model should look like this. 4 Change to the front left isometric view. Desktop Menu View ➤ 3D Views ➤ Front Left Isometric NOTE To set the viewpoint precisely, use VPOINT to specify coordinates. For example, this viewpoint is -5,-10,3. 5 Trim the body B surface with the curve that defines the upper edge of the outlet. Repeating steps 2 and 3, project wire 3 onto surface 4.
6 Trim body C with the curve that defines the lower edge of the outlet, responding to the prompts. Desktop Menu Surface ➤ Edit Surface ➤ Project Trim Select wires to project: Select wire Select wires to project: Press ENTER Select target surfaces/quilts: Select surface (6) Select target surfaces/quilts: Press ENTER 7 In the Project to Surface dialog box, specify: Direction: Normal Output Type: Trim Surface Verify that Keep Original Wires is checked, and choose OK. Your model should look like this.
To create the body D planar surface 1 Use AMJOIN3D to join the polylines that define the boundary of body D. Desktop Menu Surface ➤ Edit Wireframe ➤ Join In the Join 3D dialog box, specify: Mode: Automatic Output: Polyline Choose OK.
Your model should look like this. 4 Use CHPROP to move body D to the BODY layer. Save the file. The pump body surfaces are complete.
Creating Complex Swept Surfaces Next, you create the surfaces for the outlet on the side of the pump. outlet F (back side) outlet E outlet C outlet D outlet B outlet A Outlet A is a swept surface that blends dissimilar cross sections. To create the outlet A swept surface 1 Thaw layer 40 and make it current, and then freeze all other layers. 2 Change to the left isometric view to make lines easier to select.
4 In the Sweep Surface dialog box, in Transition, specify Scale. Choose OK. Outlet A should look like this. 5 Use CHPROP to move outlet A to the OUTLET layer. Next create a ruled surface for outlet B. The difference between this surface and the one you just completed is that outlet A is curved in two directions, and outlet B is curved in one direction and flat in the other. To create the outlet B ruled surface 1 Use AMRULE to create the outlet B surface, responding to the prompts.
Outlet B should look like this. 2 Use CHPROP to move outlet B to the OUTLET layer. Next, you create another swept surface and another ruled surface. To create the outlet C and outlet D surfaces 1 To make selections easier, rotate the model to the left with the Desktop View icons, or set specific coordinates (6,-8,1) with VPOINT, responding to the prompts. Desktop Menu View ➤ 3D Views ➤ VPOINT Current view direction: VIEWDIR=-1.0000,-1.0000,1.
Respond to the prompts: Select cross sections: Select wire (1) Select cross sections: Select wire (2) and press ENTER Select rails: Select wire (3) Select rails: Select wire (4) 1 3 4 2 5 6 3 In the Sweep Surface dialog box, under Transition, specify Scale. Choose OK. 4 Use AMRULE to create outlet D ruled surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Rule Select first wire: Select wire (5) Select second wire: Select wire (6) Your model should look like this.
To create the outlet E planar surface 1 Use AMJOIN3D to join the polylines. Surface ➤ Edit Wireframe ➤ Join Desktop Menu In the Join3D dialog box, specify: Mode: Automatic Output: Polyline Choose OK. 2 Select the polylines, responding to the prompts.
2 Select the polylines to join, responding to the prompts. Select start wire or: Select wire (5) Select wires to join: Select wire (6) and press ENTER Reverse direction? [Yes/No] : Press ENTER to accept the join direction NOTE Use the Manual mode to join lines even if they are far apart. It joins all the lines you select in the order you choose them. 3 Use AMPLANE to create outlet F from the lines you just joined, responding to the prompts.
Using Projection to Create Surfaces Next, you use projection to create ruled and planar surfaces for the base of the pump. base B base A base C To create the base A surface 1 Thaw layer 50 and make it current. Then freeze all other layers. 2 Change to the left front isometric view. Desktop Menu View ➤ 3D Views ➤ Front Right Isometric 3 Use AMRULE to create the base A surface, responding to the prompts.
The illustration shows the ruled surface fit to the flat areas and corner curves. 4 Use CHPROP to move base A to the BASE layer. Next, you join the lines needed to create a planar surface on the bottom of the pump. Then you copy the surface and trim it. To create the base B and C surfaces 1 Use AMJOIN3D to create a polyline from two wires. Desktop Menu Surface ➤ Edit Wireframe ➤ Join In the Join3D dialog box, specify: Mode: Automatic Output: Polyline Choose OK.
3 Create a planar surface on the bottom of the base, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Planar Specify first corner or [Plane/Wires]: Enter w Select wires: Select wire (1) and press ENTER The planar surface is created. 4 Use COPY to copy the last surface, responding to the prompts.
To trim the base C surface 1 Use CHPROP to move the bottom surface to the BASE layer. 2 Project the curve of the body onto the top surface of the base, responding to the prompts. Desktop Menu Surface ➤ Edit Surface ➤ Project Trim Select wires to project: Select polyline (1) and press ENTER Select target surfaces/quilts: Select surface (2) and press ENTER 1 2 3 In the Project to Surface dialog box, specify: Direction: Normal Output type: Trim Surface Choose OK. Your model should look like this.
Using Advanced Surfacing Techniques Next, you create the support rib from the surfaces. Using the techniques you have already learned, surface the support rib from these general instructions. Save a copy of your drawing before you begin working on your own. rib C rib A rib B To create the support rib 1 Thaw layer 60. 2 Create a ruled surface on the left side of the support rib (rib A). 3 Create a ruled surface on the right side of the support rib (rib B). 4 Move the surfaces to the SUPPORT_RIB layer.
To create the rib A and rib B surfaces 1 Thaw layer 60 and make it current. Then freeze all other layers. 2 Use AMRULE to create a ruled surface on the left side of the support rib, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Rule Select first wire: Select wire (1) Select second wire: Select wire (2) 1 2 3 4 3 Create a ruled surface on the right side of the support rib, responding to the prompts.
To create the rib C surface 1 Use AMSWEEPSF to create the rib C surface, responding to the prompts. Desktop Menu Surface ➤ Create Surface ➤ Sweep Select cross sections: Select wire (1) and (2) Select cross sections: Press ENTER Select rails: Select wires (3) and (4) 1 3 4 2 2 In the Sweep Surface dialog box, under Transition, specify Scale. Choose OK. Your surface should look like this. 3 Move the surface to the SUPPORT_RIB layer.
To add the support rib 1 Thaw the BODY and BASE layers. 2 Use AMPROJECT to project the support rib onto the pump, responding to the prompts. Desktop Menu Surface ➤ Edit Surface ➤ Project Trim Select wires to project: Select wire (1) and press ENTER Select target surfaces/quilts: Select surface (2) Select target surfaces/quilts: Select surface (3) and press ENTER 3 2 1 3 In the Project to Surface dialog box, specify: Direction: Normal Output: Trim Surface Choose OK.
Viewing Completed Surfaced Models To view the completed model, freeze all layers except BASE, BODY, INLET, OUTLET, SUPPORT_RIB, and TOP. Use the Zoom Extents option of ZOOM to view the entire wireframe model. One half of the pump housing is complete. You can mirror the surfaces to create a complete model.
670
Working with Standard Parts In This Chapter Standard parts is the term used for the vast selection of real-world reusable 2D and 3D parts, holes, features, and structural steel profiles that are available to you in 22 ■ Selecting standard parts ■ Inserting holes using the cylinder axial placement method ■ Inserting holes using the cylinder radial placement method Autodesk® Mechanical Desktop® 6 with the power pack.
Key Terms Term Definition base standard Predefined drafting standard that conforms to International Drafting Standards ANSI, BSI, CSN, DIN, GB, ISO, and JIS. cylinder axial Option for placement when you insert a standard part or hole parallel to a cylinder axis. cylinder radial Option for placement when you insert a standard part or hole radial into a cylinder. hole Geometric feature with a predefined shape: drilled, counterbore, or countersink.
Tutorial at a Glance This tutorial is an introduction to the standard parts and calculations functionality in Mechanical Desktop 6. You will become familiar with some of the intelligence and automation built into this functionality as you perform exercises to insert ■ ■ ■ ■ A through hole using the cylinder axial placement method. Through holes using the cylinder radial placement method. A screw connection using the automated screw connection feature. A standard related 2D-Representation of standard parts.
Inserting Through Holes It is no longer necessary to insert a workpoint on the cylinder face, dimension it, and insert a hole on the workpoint. Instead, the standard hole function automatically defines a workpoint at the location you select, dimensions it, and places the hole you specify. You can also define the insertion point dynamically. Using Cylinder Axial Placement In this exercise, you insert a standard through hole using the cylinder axial placement method.
To insert a hole using cylinder axial placement 1 Use AMTHOLE3D to define the hole to insert. Menu Content 3D ➤ Holes ➤ Through Holes In the Select a Through Hole dialog box, select ISO 273 normal. 2 In the Hole Position Method First Hole dialog box, specify: Placement: Cylinder Axial Choose OK.
4 Continue on the command line. Select radius: Press SHIFT and in the graphics area, right-click and choose Midpoint 5 Select the midpoint of the upper horizontal edge (2). 2 6 Continue on the command line.
7 In the ISO 273 normal - Nominal Diameter dialog box, specify: Select a size: M10 Choose Finish. The through hole is inserted in the size and location you selected. Save the file as md2_ex01a.dwg. Using Cylinder Radial Placement In this exercise, you insert a through hole using the cylinder radial method. Use this method to insert holes radial to a cylinder face.
To insert a hole using cylinder radial placement 1 Use AMTHOLE3D to define the hole to insert. Menu Content 3D ➤ Holes ➤ Through Holes In the Select a Through Hole dialog box, select ISO 273 normal. 2 In the Hole Position Method First Hole dialog box, specify: Placement: Cylinder Radial Choose OK. 3 On the command line, respond to the prompts as follows: Select cylindrical face: Select the upper cylindrical face (1) 1 Continue on the command line.
4 Select the midpoint of the upper vertical edge (2).
6 In the ISO 273 normal - Nominal Diameter dialog box, specify: Select a size: M10 Choose Finish. The through hole is inserted. Your drawing should look like this: Save the file as md2_ex01b.dwg.
Inserting Screw Connections In this exercise, you begin with a drawing of two parts that need a screw connection. Using the screw connection feature, you select the screw, holes, and nut that you want to use. You define the size of the screw in a dialog box. Then you insert the screw connection in the assembly. With this method, there is no need to create two separate holes before you insert the screw with the nut. The screw connection function does this for you automatically.
To insert a screw connection 1 Use AMSCREWCON3D to choose and define the screw to insert. Menu Content 3D ➤ Screw Connection In the Screw Connection dialog box, select Screws. Next, define the type of screw.
2 In the Please select a Screw dialog box, select Socket Head Types. Select the screw IS2401. The Screw Connection dialog box is displayed again. 3 Repeat steps 1 and 2 to select and define each of the following parts: Hole ➤ Through Cylindrical ➤ IS1602 normal Hole ➤ Through Cylindrical ➤ IS1602 normal Nut ➤ Hex Nuts ➤ ISO842 After you select and define the parts for the screw connection, select a size for the diameter.
4 Select M10 for the diameter. Choose Finish. The Hole Position Method First Hole dialog box is displayed. 5 In the Hole Position Method First Hole dialog box, specify the hole positioning method as follows: Placement: 2 Edges Choose OK.
6 On the command line, respond to the prompts as follows: Select first edge or planar face: Specify the first edge (1) Select second edge or planar face: Specify the second edge (2) 1 2 Continue on the command line. Specify the hole location: Specify a point on the face, offset from the two edges Enter distance from first geometry (highlighted) [Associate to/Equation assistant] <15.06>: Enter 20 Enter distance from second geometry (highlighted) [Associate to/Equation assistant] <23.
7 In the Hole Position Method Next Hole dialog box, specify: Placement: Workpoint UCS Choose OK.
The screw connection is inserted. Your drawing should look like this: You have completed this tutorial. Save the file as md6_ex17b.dwg.
688
Creating Shafts In This Chapter The shaft generator in Autodesk® Mechanical Desktop® 6 is an automated feature that eliminates the need for 23 ■ New in this tutorial ■ Using the Shaft Generator ■ Creating shaft geometry many of the manual steps previously required to create shafts. ■ Adding thread and profile information to a shaft ■ Editing a shaft In this tutorial, you learn how to design shafts using the shaft generator.
Key Terms Term Definition bearing calculation Calculates limiting value, dynamic and static load rating, dynamic and static equivalent load, and fatigue life of bearing in revolutions and hours. centerline Line in the center of a symmetrical object. When you create centerlines, you specify the start and end points. chamfer A beveled surface between two faces or surfaces. dynamic calculation Calculation required for a revolving bearing. The result is the Adjusted Rating Life.
Tutorial at a Glance It is no longer necessary to create a cylinder manually and define new sketch planes and work planes in order to create a shaft. Instead, you make selections in the 3D Shaft Generator dialog box, and enter values to further define your selections. In this tutorial you use this automated feature to ■ ■ ■ ■ ■ Create a shaft with cylindrical and conical sections. Add threads and a profile to the shaft. Edit the shaft. Add standard parts to the shaft.
Using the Shaft Generator You use the 3D Shaft Generator dialog box to select a type of shaft segment, such as a cylinder or a cone, and then you define that segment. The shaft generator creates the segment automatically and adds it to the previous segment. Getting Started In order to work through this tutorial chapter, the ISO standard system has to be installed at your system. Moreover, you need to set your measurement units to metric. This can easily be done by selecting an appropriate drawing template.
Creating Shaft Geometry You start creating the shaft by defining the segments that govern its shape. In the 3D Shaft Generator dialog box, you select the first segment type and then you define that segment. You continue adding segments until the contour of the shaft is complete. To create a shaft using the shaft generator 1 Use AMSHAFT3D to define the shaft.
3 Choose the Slope icon, and respond to the prompts as follows: Specify length or [Dialog/Associate to/Equation assistant] <10>: Enter 7 Specify diameter at start point or [Associate to/Equation assistant] <74>: Press ENTER Specify diameter at end point or [Slope/aNgle/Associate to/Equation assistant] <72>: Enter 48 NOTE If the 3D Shaft Generator dialog box hides your shaft, move the dialog box to another position on the screen.
Adding Threads to Shafts The 3D Shaft Generator dialog box provides the option to add threads to a shaft. You define the thread information in the Thread dialog box, and the thread is added to the shaft automatically. To add threads to a shaft 1 In the 3D Shaft Generator dialog box, select the Outer Contour tab and choose the Thread icon. 2 The Thread dialog box is displayed. Select ISO 261 from the available thread types.
3 The Thread ISO 261 dialog box is displayed. Specify: Nominal Diameter d [mm]: M 32 x 1.5 Length l=: Enter 12 4 Choose OK. NOTE If you have previously chosen a thread standard, the Thread dialog box opens directly to the Nominal Diameter selection screen (illustrated above). There is no need to choose the same standard again. To return to the standard selection list in the Thread dialog box, choose Standard.
Adding Profile Information to Shafts The 3D Shaft Generator dialog box provides the option to add a profile to a shaft. You further define the profile information in the Shaft dialog box. Add a profile segment to connect a drive to the shaft. To add a profile to a shaft 1 In the 3D Shaft Generator dialog box, choose the Profile icon. 2 In the Profile dialog box, select ISO 14. 3 In the Splined Shaft dialog box, specify: Nominal Size n x d x D [mm]: 6 x 26 x 30 Length l=: Enter 30 Choose OK.
5 Close the 3D Shaft Generator dialog box. The shaft contour is complete. Your drawing should look like this. Save your drawing as shaft.dwg. Next, you edit the shaft. Editing Shafts You can make changes to simple shaft segments such as cylinders and cones. It is recommended that you delete a more complex segment, such as a gear, and create a new one. In this exercise, you add a chamfer to a segment and you add a groove to another segment. First, add a chamfer to the end segment of your shaft.
To add a chamfer to a shaft segment 1 Activate the shaft generator. Menu Content 3D ➤ Shaft Generator Command AMSHAFT3D 2 On the command line, respond to the prompts as follows: Specify start point or [Existing shaft]: Enter E Select shaft: Select the shaft 3 In the 3D Shaft Generator dialog box, select the Outer Contour tab. Choose the chamfer icon, and respond to the prompts as follows: Select edge for chamfer: Select the edge (1) Specify length (max. 5) or [Associate to/Equation assistant] <2.
To insert a groove on a shaft segment 1 Choose the Groove icon, and respond to the prompts as follows: Select cylinder or cone: Select the third cylindrical section (1) Select position on cylinder or cone [Line/Plane]: Specify the point (2) Specify direction or [Flip/Accept] : Press ENTER Enter distance from base plane [Associate to/Equation assistant] <11.4>: Enter 25 Specify length or [Associate to/Equation assistant] <5>: Enter 1.
Adding Standard Parts to Shafts In Mechanical Desktop Power Pack, standard parts such as bearings, seals, circlips, keys, adjusting rings, and undercuts are available. You can select and insert these standard parts using the shaft generator. When you insert a standard part on a shaft, the standard part is not consumed by the shaft. You are actually building an assembly. An icon for each new part is displayed in the Browser under the assembly icon.
5 In the ISO 355 dialog box, verify Geometry is selected and specify: Inner Diameter: 40 Choose Next to continue. You use the ISO 355 dialog box for the bearing calculation. 6 In the ISO 355 dialog box, verify Calculation is selected and specify the values as shown below. By choosing dynamic calculation, Mechanical Desktop is calculating the adjusted rating life of the bearing. Choose Next. The possible bearings are calculated and the results are displayed in the ISO 355 dialog box in Result.
7 In the ISO 355 dialog box, select the Result tab, and then select 2BC - 40 x 62 x 15. Choose Finish. Use dynamic dragging to size the bearing on the screen. 8 Respond to the prompt as follows: Drag size [Dialog] <10>: Drag the bearing, and click when 2BC - 40 x 62 x 15 is displayed in the status bar The bearing is inserted and your drawing should look like this. Insert a second bearing, starting from the groove at the left of the fifth segment of the shaft.
To add the second bearing 1 In the 3D Shaft Generator dialog box, choose Std. Parts. 2 In the Select a Part dialog box, choose Roller Bearings ➤ Radial ➤ ISO 355.
Displaying and Shading 3D Views You can split your screen to display the front and isometric views of the shaft in separate viewports. You can activate a viewport by clicking inside its border. To display front and isometric views in a split screen 1 On the command line, enter 2, and press ENTER. Your drawing area is split to display front and isometric views in separate viewports. 2 Click a viewport to activate it. 3 Use AMDT_TOGGLE_SHADWIREF to add shading to the shaft.
To change the color of a single part on a shaft 1 In the Desktop Browser, right-click a bearing and choose Properties ➤ Color. 2 Select a different color. The bearing is displayed in a different color on the shaft. Try changing the colors of the other parts on the shaft. Save your file.
Calculating Stress on 3D Parts In This Chapter Autodesk® Mechanical Desktop® 6 Power Pack includes a feature called 3D finite element analysis (FEA). FEA is 24 ■ New in this tutorial ■ Using 3D FEA calculations ■ Defining loads used to calculate deformation and stress conditions on 3D parts. The 3D FEA calculations feature is a reliable ■ Calculating and displaying the result tool that helps you meet the demands of today’s sophisticated mechanical engineering.
Key Terms Term Definition distributed force A force that is spread over an area. FEA Finite element analysis. A calculation routine, or method. Calculates stress and deformation in a plane for plates with a given thickness, or in a cross section with individual forces, stretching loads, and fixed and/or moveable supports. The FEA routine uses its own layer group for input and output. fixed support A support that is fixed to a part and cannot be moved. load Forces and moments that act on a part.
Tutorial at a Glance The 3D FEA calculations feature is a simple tool that eliminates the need for the complex programs and calculations previously required to perform stress and deformation calculations. In this tutorial, you learn to use 3D FEA for calculations as you ■ ■ ■ ■ Start a finite element analysis. Define stress loads. Generate a mesh. Calculate and display the result.
Using 3D FEA Calculations To begin calculating the stress conditions on your model, you open the FEA Calculation 3D dialog box. You work in this dialog box to choose the types and quantity of loads and supports, and to define the loads and boundary conditions. Before you perform the calculation, you create a mesh on your 3D part. This mesh is required to display the results of the calculation. The calculation is displayed on your model using isoareas that define the limits of the stresses and deformations.
To start a finite element analysis 1 Use AMFEA3D to perform the FEA calculation. Menu Content 3D ➤ Calculations ➤ FEA Respond to the prompt as follows: Select 3D-Body: Select the 3D part The FEA Calculation 3D dialog box is displayed. NOTE If the FEA Calculation 3D dialog box hides your drawing, move the dialog box to another position on the screen. Defining Supports and Forces Next, you define the supports and forces that act on your part. These definitions are used for the FEA calculations.
To define supports and forces on a part 1 In the FEA Calculation 3D dialog box, choose the Face Support icon and respond to the prompts as follows: Select a surface: Click the edge (1) of the surface Specify face [Accept/Next] : Press N to cycle to the surface you selected, then press ENTER 1 NOTE You may prefer to turn OSNAP off before you create and constrain the work point. Click the OSNAP button at the bottom of your screen. The Define Border for Load, Support dialog box is displayed.
2 In the Define Border for Load, Support dialog box, choose Whole Face. Respond to the prompts as follows: Define insertion point for main symbol: Specify point or [Dialog]: Specify a point, other than an edge, on the selected face NOTE If the support does not act on the whole face, you can define an area using the different options. See the Help for more information.
4 In the Define Border for Load, Support dialog box, choose Whole Face, and respond to the prompts as follows: Define insertion point for main symbol: Specify point or [Dialog]: Specify a point, other than an edge, on the selected face 5 In the FEA Calculation dialog box, choose the Face Force icon and respond to the prompts as follows: Select a surface: Click the edge (3) of the surface Specify face [Accept/Next] : Press N to cycle to the surface you selected, then press ENTER 3 The Define Border
You have the defined the border conditions for two supports and one force. Your drawing should look like this: Calculating and Displaying the Result Continue in the FEA Calculation 3D dialog box to perform the calculations and display the results. Before you can calculate and display the result, you need to generate a mesh. To generate a mesh 1 In the FEA Calculation 3D dialog box, under Run Calculation, turn on Auto Refining. 2 Choose the Run Calculation icon.
Continue in the FEA Calculation 3D dialog box to calculate surface isoareas and deformation. 4 Under Results, choose the Isolines (Isoareas) icon. 5 In the Surface Isolines (Isoareas) dialog box, choose the Isoareas button, and choose OK. Your model with isoareas is displayed on the screen beside the model with mesh.
7 In the Deformed Mesh dialog box, turn on Automatic, and choose OK. Respond to the prompts as follows: Specify base point or displacement : Enter 150,150 Specify second point of displacement: Press ENTER Specify insertion point or [Paper space]: Specify a suitable location for the table near the mesh display 8 Close the FEA Calculation 3D dialog box. The calculations are finished, and the results are displayed.
718
Toolbar Icons A In This Appendix Use this appendix as a guide to using the Autodesk® Mechanical Desktop® toolbar icons. For an overview of ■ Desktop Tools toolbar icons ■ Part Modeling toolbar icons ■ Toolbody Modeling toolbar the toolbars and the Mechanical Desktop interface, refer to “Mechanical Desktop Interface” on page 17 in chapter 3.
Desktop Tools If you are working in the Part Modeling environment, the Desktop Tools toolbar contains three icons that activate the Part Modeling, Toolbody Modeling, and Drawing Layout toolbars. Part Modeling Toolbody Modeling Drawing Layout If you are working in the Assembly Modeling environment, the Desktop Tools toolbar contains four icons that activate the Part Modeling, Assembly Modeling, Scene, and Drawing Layout toolbars.
Part Modeling The Part Modeling toolbar provides the tools you need for creating and modifying parts.
Part Modeling ➤ New Sketch Plane New Sketch Plane Sketch View Highlights Sketch Data Part Modeling ➤ 2D Sketching Launches 2D Sketch Toolbar Construction Line Construction Circle Polyline Line Arc 3 Points Flyout Spline Rectangle Polygon Circle Flyout Copy Object Mirror Offset Move Trim Extend Fillet Object Snaps Flyout Erase Single Profile Sketch Flyout Re-Solve Sketch Append to Sketch Launches 2D Constraints Toolbar 722 | Appendix A Toolbar Icons
Part Modeling ➤ 2D Sketching ➤ Arc 3 Points Arc 3 Points Arc Start Center End Arc Start Center Angle Arc Start Center Length Arc Start End Angle Arc Start End Direction Arc Start End Radius Arc Center Start End Arc Center Start Angle Arc Center Start Length Arc Continue Part Modeling ➤ 2D Sketching ➤ Circle Circle Center Radius Ellipse Center Part Modeling | 723
Part Modeling ➤ 2D Sketching ➤ Object Snaps Snap to Endpoint Snap to Tangent Snap to Apparent Intersect Snap to Center Part Modeling ➤ 2D Sketching ➤ Sketch Profile 2D Path 3D Path Break Line Cut Line Split Line Text Sketch Copy Sketch Copy Edge Project to Plane 724 | Appendix A Toolbar Icons
Part Modeling ➤ 2D Constraints Launches 2D Constraints Toolbar Show Constraints Delete Constraint Tangent Concentric Collinear Parallel Perpendicular Horizontal Vertical Project Join X Value Y Value Radius Equal Length Mirror Fixed Power Dimensioning Flyout Power Edit Flyout Re-Solve Sketch Append to Sketch Design Variables Launches 2D Sketch Toolbar Part Modeling | 725
Part Modeling ➤ 2D Constraints ➤ Power Dimensioning Power Dimensioning New Dimension Part Modeling ➤ 2D Constraints ➤ Power Edit Power Edit Edit Dimension Part Modeling ➤ 2D Constraints ➤ Design Variables Design Variables Display as Variables Display as Numbers Display as Equations Part Modeling ➤ Profile a Sketch Profile Single Profile 2D Path 3D Path Break Line Cut Line Split Line Text Sketch Re-Solve Sketch Append to Sketch Copy Sketch Copy Edge 726 | Appendix A Toolbar Icons
Part Modeling ➤ Sketched Features Extrude Revolve Sweep Loft Rib Bend Face Split Part Modeling ➤ Placed Features Hole Thread Face Draft Fillet Chamfer Shell Surface Cut Rectangular Pattern Polar Pattern Axial Pattern Copy Feature Combine Part Split Part Modeling ➤ Work Features Work Plane Work Axis Work Point Create Basic Work Planes Part Modeling | 727
Part Modeling ➤ Power Dimensioning Power Dimensioning New Dimension Power Edit Edit Dimension Part Modeling ➤ Edit Feature Edit Feature Reorder Feature Suppress Features Suppress by Type Unsuppress Features Unsuppress Features by Type Table Driven Suppression Access Delete Feature Part Modeling ➤ Update Part Update Part Update Assembly Feature Replay 728 | Appendix A Toolbar Icons
Part Modeling ➤ Part Visibility Part Visibility Unhide All Unhide Pick Display All Work Planes Display All Work Axes Display All Work Points Display All Cut Lines Hide All Hide All Except Hide Pick Part Modeling ➤ Options Part Options List Part Mass Properties Design Variables Part Modeling | 729
Toolbody Modeling In the Part Modeling environment, the Toolbody Modeling toolbar contains the tools you need to create combined parts.
Toolbody Modeling ➤ 3D Toolbody Constraints Launch 3D Constraints Toolbar Mate Flush Angle Insert Edit Constraints DOF Visibility Update Positioning Design Variables Toolbody Modeling ➤ Power Manipulator Power Manipulator List Part Data Toolbody Modeling ➤ Check Interference Check 3D Interference Audit External Refs Update External Refs Minimum 3D Distance Toolbody Modeling | 731
Toolbody Modeling ➤ Toolbody Visibility Toolbody Visibility Unhide All Unhide Pick Display All Toolbodies Display All CGs Display All DOFs Hide All Toolbody Objects Hide All Except Hide Picked Toolbody Objects Assembly Modeling In the Assembly Modeling environment, the Assembly Modeling toolbar provides the tools you need to create and modify assemblies and subassemblies.
Assembly Modeling ➤ New Subassembly New Subassembly Activate Assembly Assembly Modeling ➤ Assembly Catalog Assembly Catalog Detach Part/Assembly Replace Part Where Used? Input Part Definition Output Part Definition Assembly Modeling ➤ 3D Assembly Constraints Launch 3D Constraints Toolbar Mate Flush Angle Insert Edit Constraints DOF Visibility Update Assembly Design Variables Assembly Modeling | 733
Assembly Modeling ➤ Assign Attributes Assign Attributes Hatch Patterns Assembly Modeling ➤ Power Manipulator Power Manipulator List Part Data Assembly Modeling ➤ Mass Properties Mass Properties Check 3D Interference Audit External Refs Update External Refs Minimum 3D Distance Assembly Modeling ➤ Assembly Visibility Assembly Visibility Unhide All Unhide Pick Display All Parts Display All Assemblies Display All CGs Display All DOFs Hide All Assembly Objects Hide All Except Hide Picked Assembly Objects 734
Surface Modeling The Surface Modeling toolbar provides the tools you need to create and modify 3D wireframe surfaces. To activate the Surface Modeling toolbar, choose Surface ➤ Launch Toolbar.
Surface Modeling ➤ Swept Surface Swept Surface Extruded Surface Tubular Surface Revolved Surface Surface Modeling ➤ Loft U Surface Loft U Surface Loft UV Surface Ruled Surface Planar Surface Planar Trimmed Surface Surface Modeling ➤ Blended Surface Blended Surface Offset Surface Fillet Surface Corner Fillet Surface 736 | Appendix A Toolbar Icons
Surface Modeling ➤ Flow Wires Flow Wires Section Cuts Augmented Line Copy Surface Edge Parting Line Intersection Wire Projection Wire Offset Wire Create Tangent Spline Surface Modeling ➤ Object Visibility Object Visibility Unhide All Unhide Pick Hide All Hide All Except Hide Pick Surface Modeling ➤ Surface Display Surface Analysis Surface Display Surface Mass Properties Surface Modeling | 737
Surface Modeling ➤ Stitches Surfaces Stitches Surfaces Surface Thicken Adjust Replace Surface Edge Solid Cut Convert Face Convert All Surface Modeling ➤ Grip Point Placement Grip Point Placement Flip Surface Normal Refine Surface Intersect and Trim Project and Trim Surface Modeling ➤ Lengthen Surface Lengthen Surface Truncate Surface Break Surface Join Surfaces 738 | Appendix A Toolbar Icons
Surface Modeling ➤ Extract Surface Loop Extract Surface Loop Copy Surface Edge Show Edge Nodes Project and Trim Delete All Trim Surface Modeling ➤ Edit Augmented Line Edit Augmented Line Add Vectors Copy Vectors Rotate Vectors Blend Vectors Vector Length Twist Vectors Delete Vectors Surface Modeling ➤ Wire Direction Wire Direction Check Fit Refine Wire Fillet Wire Join Wire Create Fitted Spline Unspline Spline Edit Surface Modeling | 739
Scene In the Assembly Modeling environment, the Scene toolbar provides the tools you need to create, modify, and manage scenes.
Scene ➤ Scene Visibility Scene Visibility Unhide All Unhide Pick Display All Parts Display All Assemblies Display All Trails Hide All Scene Objects Hide All Except Hide Picked Scene Objects Drawing Layout The Drawing Layout toolbar provides the tools you need to create, modify, and annotate drawing views and layouts.
Drawing Layout ➤ Power Dimensioning Power Dimensioning Reference Dimension Automatic Dimension Power Edit Edit Dimension Move Dimension Align Dimension Flyout Welding Symbol Flyout Line Text Flyout Annotation Flyout Dimension Style Flyout Edit BOM Database Drawing Layout ➤ Power Dimensioning ➤ Edit Format Align Dimension Join Dimension Insert Dimension Break Dimension Drawing Layout ➤ Power Dimensioning ➤ Welding Symbol Welding Symbol Surface Texture Feature Control Frame Datum Identifier Datum Target F
Drawing Layout ➤ Power Dimensioning ➤ Line Text Line Text Multiline Text Edit Text Drawing Layout ➤ Power Dimensioning ➤ Annotation Annotation Leader Hole Note Flyout Centerline Drawing Layout ➤ Power Dimensioning ➤ Edit BOM Database Edit BOM Database Place Balloon Place Reference Place Parts List Part Reference Edit Edit Part List/Balloon Drawing Layout | 743
Drawing Layout ➤ Drawing Visibility Drawing Visibility Unhide All Unhide Pick Display All Viewports Display All Parts Lists Display All Balloons Display All Reference Dims Display All Parametric Dims Hide All Drawing Objects Hide All Except Hide Picked Drawing Objects Mechanical View The Mechanical View toolbar provides the tools you need to manage the view of your design, control 3D viewports, and create rendered views of your parts and assemblies.
Mechanical View ➤ Zoom Realtime Zoom Realtime Zoom All Zoom In Zoom Out Zoom Previous Zoom Window Mechanical View ➤ 3D Orbit 3D Orbit New Rotation Center Select Rotation Center Lighting Control 3D Continuous Orbit 3D Pan 3D Zoom 3D Swivel 3D Adjust Distance 3D Adjust Clip Planes Front Clip On/Off Back Clip On/Off Mechanical View | 745
Mechanical View ➤ Sketch View Sketch View Top View Bottom View Left View Right View Front View Back View Left Front Isometric View Right Front Isometric View Left Back Isometric View Right Back Isometric View Mechanical View ➤ Restore View #1 Restore View #1 Restore View #2 Restore View #3 Save View #1 Save View #2 Save View #3 Named Views Single Viewport Two Viewports Three Viewports Four Viewports 746 | Appendix A Toolbar Icons
Mechanical View ➤ Toggle Shading/Wireframe Toggle Shading/Wireframe 2D Wireframe 3D Wireframe Hidden Flat Shaded Gouraud Shaded Flat Shaded, Edges On Gouraud Shaded, Edges On Mechanical View | 747
748
Index A active part variables, 362 adjusting surfaces, 569 ambient light on images, 304 Angle type dialog box, 714 angular dimensions, 92 annotations, 337 Approximate Model Size dialog box, 624 array features, editing, 223 assemblies analyzing, 506 completing, 497 restructuring, 479, 504 thumbnail previews, 483 updating, 509 Assembly Catalog, 377, 400, 403, 482 Assembly Mass Properties dialog box, 419, 510 assembly modeling checking interference, 418, 506, 510 concepts, 401, 479 constraints, 407, 414, 438,
constraints (continued) dimension, 94 displaying, 96 displaying symbols, 90 equal length, 110 fix, 51, 88, 97 flush, 478 geometric, 84, 88, 94, 272 hiding, 51 insert, 400 mate, 400, 407 missing, 113 modifying, 91, 414, 438 path sketch, 111 project, 107, 276 radial, 102 sketch, 42, 49, 86, 128, 175, 260 techniques, 119 toolbody parts, 454 construction geometry, 42, 105 controlling tangency, 115 dimensioning circles, 118 in path sketches, 111 lines, 107 consumed sketches, 122, 254 Context Menu command access,
Loft Surface, 556 Mechanical Options, 49, 524, 624 Mechanical Options, Part, 54 Nominal Diameter, 677 Note Symbol, 334, 335, 394, 395 Object Grouping, 558 Page Setup, 426 Part Catalog, 444, 449 Part Ref Attributes, 526 Paste Special, 397 Pattern, 216 Please select a Screw, 683 Plotter Configuration Editorial, 427 Polyline Fit, 550 Power Dimensioning, 330 Power Manipulator, 422, 516 Project to Surface, 574, 637 Properties for ANSI, 524 Revolution, 150, 176, 289 Rib, 136 Screw Connection, 682 Select a Part, 7
F Face Draft dialog box, 194 face drafts, 186, 194 faces on shells, 346 excluding, 353 faces, splitting, 152 FEA Calculation 3D dialog box, 709, 711 features, 42, 122 appending to tables, 373 arrays, editing, 223 base, 122, 123, 254, 257, 258, 578 bend, 46, 163 chamfering, 204 combine, 444, 457, 458 combining, 186, 227 controlling shapes of, 235 copying, 224 creating from surfaces, 577 cutting, 350, 605 embossing, 140 extruding, 124, 130, 182, 262, 586 filleting, 186 hole, 188, 598 lofting, 122, 143, 145 mo
loads on parts, 708 local parts, 400, 478, 481 Loft dialog box, 144 Loft Surface dialog box, 556 lofted features, 122, 143 lofted surfaces, 555 lofting cubic, 145 linear, 143 logical surface areas, 614, 616 M Manual mode vs.
polar patterns, 218 Polyline Fit dialog box, 550, 552 polylines, 619, 629, 642, 643 power dimensioning, 330, 390 Power Dimensioning dialog box, 330 Power Manipulator dialog box, 422, 516 preferences, surface, 624 profile planes, 234 profile sketches, 71, 127, 258, 270, 282, 586, 588 closed, 46 collinear, 592 constraining to work points, 181 construction geometry, 105 examining, 96 extruding to plane, 172 open, 46 revolving, 175 single, 597 text-based, 45 profiles, adding to shafts, 697 project constraints,
sketching (continued) on planes, 594, 601 process, 255 profile, 42, 96, 105, 127, 270, 586, 588, 592 restoring shapes of, 595 rough, 49 rules, 47, 55 single profiles, 106, 597 spline path, 70 split line, 42, 77 text sketch profiles, 42, 45 tips, 44 tolerances, 42, 54 skin surfaces, 534, 546 Splined Shaft dialog box, 697 splines, 576 split lines, 42, 77, 154, 229 spreadsheets linking, 362 pasting into drawings, 396 standard parts, 672 adding to shafts, 701 holes, through, 674 standards, base, 672 start angle
taper angles for sweeps, 234 Text Sketch dialog box, 141 text sketch profiles, 42, 45 thickness overrides, 346, 356 thin features, 46, 136 thread, defining, 695 three-dimensional edge paths, 160 helical paths, 65, 157 path sketches, 62, 71 pipe paths, 67, 161 spline paths, 70, 162 through termination, 672 tips constraining, 86 sketching, 44 title blocks, inserting, 428 toolbodies, 444 attaching, 449 combining, 453, 458, 463 constraining, 462 consumption of, 444 copying definitions, 451 localizing external,
